Archive for year: 2017

December 15, 2017
15 Dec 2017

MecSoft Releases RhinoCAM & VisualCAD/CAM 2018

Irvine, CA, Dec 18, 2017: MecSoft Corporation, the developer of industry leading CAD/CAM software solutions, has announced the availability of the following products

  • RhinoCAM 2018, the newest version of MecSoft’s integrated CAM solution for Rhinoceros 5.0
  • VisualCAD/CAM 2018, the latest version of their flagship standalone CNC programming software

Release Highlights

  • 2 ½ Axis – Automatic Feature Detection & Automatic Feature Machining
  • 3 Axis – Horizontal Finishing follow containment, performance & stability improvements
  • 4 Axis – Create Round Stock method & Helical Milling
  • 5 Axis – Use 5 Axis continuous programming methods for 4 axis machining
  • CAM Application Programming Interface in RhinoCAM
  • NEST & ART modules now are included free of cost in all MILL configurations

The newly released Automatic Feature Detection (AFD) & Automatic Feature Machining (AFM), along with an Application Programming Interface (API), provide powerful new automation tools to our CAM customers. Coupled with new toolpath methods and enhancements to existing methods, MecSoft continues to deliver outstanding value to our customers.”, stated Joe Anand, President and CEO of MecSoft Corporation.

Free demo software of VisualCAD/CAM 2018 can be downloaded at MecSoft.com.

About MecSoft Corporation

Headquartered in Irvine, California, MecSoft Corporation is a worldwide leader in providing Computer Aided Manufacturing (CAM) software solutions, addressing both Additive and Subtractive manufacturing technologies, for the small to mid-market segments. These solutions include products VisualCAD/CAM/3DPRINT®, VisualCAM for SOLIDWORKS® and RhinoCAM™ & Rhino3DPRINT. These software products deliver powerful, easy-to-use and affordable solutions for users in the custom manufacturing, rapid prototyping, rapid tooling, mold making, aerospace, automotive, tool & die, woodworking, and education industries.

For the latest news and information, visit mecsoft.com or call (949) 654-8163.

December 4, 2017
04 Dec 2017

The Tamiya Porsche Turbo RSR Type 934 Wheel Kit

Just like installing aftermarket components on a new automobile, scale model kit enthusiasts can purchase and install aftermarket components for their scale model kits. This allows them to change the look and style of their original model kit. Jim Orth, owner/operator of Riverview Hobbies, LLC uses Rhino and RhinoCAM to design and program the CNC toolpaths required to machine single and multi-cavity molds for their aftermarket kits. Read the complete case study here.

This wheel kit is designed specifically for the 1/12 Tamiya Porsche Turbo RSR Type 934. It offers builders an easy to use contemporary wheel option for their Street and Tuner builds. The 1/12 scale resin wheels replace Tamiya kit parts L2 and L8 without any modifications to adjacent parts or changes in wheel mounting technique. Look at the accuracy and attention to detail on display in the 25 cap head screws around the wheel rim!

“Why do we use RhinoCAM? It’s cost-effective, accurate and not difficult to understand! I like the integration between Rhino and RhinoCAM – it allows a workflow where changes in the design process are immediately visible to the CAM toolpaths which is invaluable. Plus your tech support is always there when I need help. The close relationship we have developed over the years means a lot to me. I’m very happy with RhinoCAM!”

Jim Orth, Owner/Operator, Riverview Hobbies, LLC

The kit includes 4 inner wheel sleeves and wheel faces (outer chrome wheel sleeves from the Tamiya kit are required) along with 4 hub adapters sized for the front and rear axles (2 front and 2 rear). Also included are 3 optional resin wheel center treatments; an exposed axle nut, dust cap or full cover center cap along with 4 resin valve stems. Here is a look at the wax mold, kit components and final assembly.

The Porsche 934 wheel kit wax mold half machined from RhinoCAM toolpaths.

The Porsche 934 wheel kit components.

The production Porsche 934 Wheel Kit tooling in resin

The Tamiya Porsche Turbo RSR Type 934 with Wheel Kit assembled

More About Riverview Hobbies

We would like to thank Jim Orth, Owner/Operator of Riverview Hobbies for allowing us to share their RhinoCAM success story! For more information about Riverview Hobbies and their complete line of aftermarket kits we invite you to visit them online at riverviewhobbies.com.

November 27, 2017
27 Nov 2017

Best Practices in 2½ Axis Machining

2½ Axis machining is the 2nd most common application (behind 3 Axis machining) for all of MecSoft’s CAM plugins. The reason for this is because a large number of parts found in the real world lend themselves to 2½ Axis machining. The majority of 2½ Axis components are simple prismatic shapes composed of drilled holes, flat horizontal faces and straight or drafted verticals walls.

In 2½ Axis machining the cutter moves in a plane in both the X and Y direction while maintaining a fixed Z height. The ½ axis is appended to 2 Axis, to denote the fact that cutting is done in successive fixed Z height planes starting at the highest Z level and stopping at a lowest Z level, thereby machining a complete 3D prismatic part. This method of machining is not quite 3 Axis where all three axes (X,Y and Z) can be continually changed when machining. 

In this post we’ll explore Best Practice methods and understanding for machining components using the following 2½ Axis toolpath strategies in MecSoft CAM:

  • Facing
  • Pocketing
  • Profiling
  • Engraving
  • Hole Pocketing
  • Hole Profiling

If you also machine in 3 Axis or plan to in the future, be sure to check out our blog post Best Practices in 3 Axis Machining!

 

CAD Geometry & File Formats

Similar to 3 Axis your CAD geometry plays an important role in 2½ Axis machining. Most importantly here, is making the determination that 2½ Axis machining strategies are indeed the best approach. You can only make this determination by reviewing and understanding the part geometry.

At a minimum you need 2D geometry such as lines and arcs (we’ll just call them curves) to machine in 2½ Axis. These curves would lie on a plane parallel to the XY plane and can be at any Z height. However, having an actual 3D model is even better because it allows you to both visualize the part and the machining processes at the same time. In some cases you may want to use a combination of both 2½ Axis and 3 Axis toolpath strategies. In other cases, you can save time by simply using a 3 Axis toolpath strategy.

If your part contains ANY contours that would require the cutting tool to move simultaneously in all three X, Y and Z axis, you MUST use 3 Axis machining strategies.


For recommendations on CAD File Formats you can refer to our
Best Practices in 3 Axis Machining blog post. 

3D Part in SolidWorks Designer

3D Part in Rhino Modeler

 

2D Drawing in VisualCAD (shown with stock displayed)

Best Practices

Here are some things to consider regarding CAD Geometry and File Formats specifically for 2½ Axis machining:

  1. 3D is always better than 2D:
    If given a choice always ask for the 3D solid part model. It will remove all ambiguity thereby allowing you to better evaluate the part and your machining job requirements. Native files created from the same CAD system where you are running MecSoft CAM as a plug-in are preferred. If this is not possible, ask for the 3D part in both STEP (*.stp) and IGES (*.igs) file formats. Refer to our
    Best Practices in 3 Axis Machining blog post for more specific recommendations on CAD Geometry and File Formats.

  2. When curves are better than lines:
    If the part has ANY curved edges make sure the CAD file includes actual curve geometry such as arcs, circles, splines, etc. and not just line segments. Avoid SLA and STL file formats if possible.
  3. Think Vector, not Raster:
    For 2D geometry, vector drawings (i.e., lines, arcs and curves) are required. You can use DWG and DXF files for this purpose. These are AutoCAD® drawing formats so files from the later versions are better. Raster files are bitmap image files and
    ARE NOT machinable.

General Machining Checklist

Before you start any toolpath project ask yourself these questions. Knowing the answers before you start can save you time and money down the road.

  1. Are the Units, Size and Orientation correct?
    Check your part file to make sure it is in the expected units (MM or Inches). Check the size of your part. You can do this quickly by selecting the Stock icon from the Machining Job tree. Check to make sure the part is oriented correctly for machining.
  2. Will the part fit on my CNC machine? 
    If not, can you machine it in sections? Also, can you machine all of the required features from one side or will a secondary setup and machining be required?
  3. Is this a 2½ Axis Part? 
    If your part has tapered walls then 3 Axis toolpaths may be required. Note that some simple tapered walls can be machined with tapered cutters. So care needs to be taken when evaluating whether a part can be machined purely with 2½ Axis methods.
  4. Can I save time using 3 Axis Toolpaths? 
    Your part may have many prismatic features that can all be machined using one 3 Axis Horizontal Roughing strategy. With Tolerances set to a finishing value such as 0.001, Stock set to zero and Clear Flats enabled, this 3 Axis toolpath strategy can perform 2½ Axis Facing, Pocketing and Profiling all at the same time. For some parts this is ideal.

Effect of Machining Tolerances

We strongly recommend that you take some time to read our previous post Best Practices in 3 Axis Machining and How to Increase Toolpath Accuracy where we cover the Effect of Machining Tolerances in greater detail. The recommendations we make below apply specifically to your 2½ Axis machining projects. 

 

Best Practices

Specifically for 2½ Axis machining here are some things to consider:

1. Pay attention to the Global Tolerance:
Machine tools have the ability to follow only two types of curves exactly as defined in ISO 6983, the international standard for numerical control which defines the data format for positioning, linear motions and contouring control systems. These curves are Lines and Arcs (Helixes are included here). Any other type of curve is followed only to the Tolerance accuracy specified in the Global Parameters section of the operation dialog. 

Why is this tolerance required?
Because the kinematic joints of a CNC machine tool cannot allow exact conformance to any other type of geometry. So free-form curves as well as other conics such as parabolas, ellipses etc. can only be followed by using a linearized representation of these curves.

2. Use of Arc Fitting:
Facing, Pocketing and Profiling supports Cut Arc Fitting. This is located on the Advanced Cut Parameters tab of the operation dialog. It allows you to fit arcs to consecutive curve segments that lie on the XY plane. The parameter has a Fitting Tolerance (t) value. It defines the maximum deviation of each chord or segment of the original linearized toolpath to the fitted arc. 

Arc Fitting Tolerance value recommendation:

This value should be 2 times the toolpath Global Tolerance value for the toolpath to allow enough room for the program to fit 3 consecutive points to an arc motion. So for example, if your resulting toolpath must be within 0.001” of the CAD geometry, set your arc Fitting Tolerance (t) to (0.001) and your toolpath operation Global Tolerance to ½ of that (0.0005”). A value lower than this may not find any linear segments to fit arcs to. A value higher than this may result in arc motions that exceed your tolerance requirements.

 

The Role of Stock to Leave

The Stock value in 2½ Axis machining applies to the extents of the cutter paths in the XY plane at each cut level. In the Pocketing operation shown in the illustration below for example, you can clearly see that the Stock value applies to the vertical walls around the perimeter of each pocket. The in-process stock model is shown transparently on top of the part model. The Z depth of the cutter is controlled by the Cut Levels tab of each operation. Refer to the Effective use of Cut Levels & Machining Regions section below for specific recommendations regarding the Z Axis.

In these pocketing operations a positive Stock value of 0.025” was specified.


Best Practices

Here are some best practices regarding stock in 2½ Axis machining:

1. Use of Bridges & Tabs:
Bridges & Tabs are used to prevent the cut piece from falling out or moving as it is being cut. This typically happens when cutting flat sheets of material like paneling. Even if you have a vacuum table to hold down parts, you may want to use Bridges & Tabs to give your stock added stability during machining. The size of the tabs will depend on your stock material. Cutting wood will require larger tabs while tabs for cutting metal can be smaller. Tabs can be positioned automatically or manually. You will need to consider how you plan to remove the excess tabs after machining.

The the height and width of Bridges & Tabs can be defined and placed automatically or manually using bridge points.


2. Stock applies to the XY Plane:

Remember that the Stock value on the Cut Parameters tab of the toolpath operation dialog refers to the vertical sides of the cutting tool as it moves in the XY plane. It determines how much stock to leave or remove in relation to the machining regions selected for the operation. Use the Cut Levels tab to adjust any stock to leave in the Z axis.

3. Minimize your Stock Size:
Use minimum stock sizes when possible. This will save both material and machining time.

4. Using a Negative Stock Value:
If your CAD geometry does not account for fit, you can use positive and negative stock in conjunction on mating parts to achieve the fit desired during assembly (press fit, slip fit, etc.). 

5. For Roughing and Finishing:
2½ Axis operations can be used for both Roughing and Finishing by simply adjusting the amount of Stock to leave. For finishing operations, the stock value is typically set to zero so as to produce the desired part geometry.

 

Effective Use of Cut Levels & Machining Regions

We mentioned previously that in 2½ Axis machining the cutter moves in the XY Plane while maintaining a fixed Z depth. The Z depth for each XY pass in relation to your selected Machining Regions is controlled using the Cut Levels tab of the operation dialog. An understanding of how cut levels are controlled is essential. 

We recommend that you review our blog post Understanding Cut Levels in 2½ Axis Machining where we go into this topic in detail.

Best Practices

Here are some best practice methods regarding Cut levels and Machining Regions in 2½ Axis machining:

1. Understand the Location of Cut Geometry:
Location of Cut Geometry refers to the machining regions you have selected in the Control Geometry tab for the operation. It is essential that you understand where this geometry is located in relation to the starting Z level of the cut. Ask yourself
“Where is my Cut Geometry?” The available options are At Top, At Bottom and Pick Top.

 

2. Know when to use the Pick Top option:
If you are machining from 2D geometry then you may be in a situation when the Pick Top option is required. In the example shown below there is no 3D model. The Control Geometry is a 2D drawing located on the XY plane at Z0 (zero). You are looking at the resulting stock after the pocket is cut. Notice that the Stock Height and the Pick Top value are the same (0.5). Pick Top allows you to tell the system where to start the Z level cut.



3. Understand your Part Region Heights:
Your machining regions might not all be on the same Z level! This can occur when you have islands within regions that are located at different levels. The example part shown below has an island that is lower than the perimeter of the pocket. The Clear Island Tops option on the Cut Levels tab allows you to add a cut level to clear this area.

Nested Machining Regions at different Cut Levels

Do not Clear Island Tops

Clear Island Tops


4. Use Rough & Finish Depths:
You can use the Cut Levels tab to automatically divide your cut levels into a Rough Depth and a Finish Depth, each with their own unique Depth/Cut values.

Use Rough & Finish Depths in the same toolpath operation

 

5. To save time, use 3D Model to Detect Depths:
If your part is a 3D solid or surface model, you can save time by checking the box to Use 3D Model to Detect Depth on the Cut Levels tab. Then just set your Depth/Cut values.

6. Understand how Radiused Mills behave near an edge:
It is important to understand how Z heights AND the XY perimeter of each machining region are honored by radiused cutting tools. We have reduced the cut level in the following example to illustrate the
waterfall effect of the Ball Mill tool as it makes contact with the edge of the machining region.

The waterfall effect of cut levels and radiused cutting tools.

7. The proper use of Avoid Regions:
Avoid Regions are typically used to avoid objects such as clamps and fixtures. When using Avoid Regions make sure they overlap the Machining Regions as shown in the examples below. They can be selected from the Avoid Regions tab on the Control Geometry section of the Facing, Pocketing and Profiling toolpath dialog.

 

8. Understand Nested Machining Regions:
When regions are nested inside one another, it is important to realize where the cutter will machine. When using a Pocketing toolpath, the system treats any nested region as islands and will cut anything between the outer pocket region and any of its inner nested islands. 


On the machining regions shown below, the nested inner regions become islands within the outer pocket region and the cutting area is shown hatched. In addition to this, if another region is nested inside of an island region, as shown below, it will be treated as a pocket region. The system applies the same rule to any depth of nesting. 

9. Optimize your Feed Rates:
There will be instances when you may not want the cutting tool to accelerate at the full Cut Feed value you have assigned for either the tool or the toolpath operation. The table below lists a few of these conditions and how to control them. See our blog post Feed Rates Explained – Extend the Life of Your CNC Tools and Machines for more detailed information on feed rates.

Conditions Controls
When plunging between Cut levels Located on the Feed Rate Reduction Factors section of the Feeds & Speed tab for both the tool and the operation
During the first XY pass when the full width of the tool is engaged in material
At sharp corners Select Feedrate Optimization from the Global Edits tab of the Toolpath Editor (Professional & Premium configurations)

 

Applying 2½ Axis Toolpath Strategies

In most cases your part geometry will dictate which 2½ Axis toolpath strategy to use. For example, if your part has profiles, pockets, holes, chamfers, etc. Also, most 2½ Axis toolpath strategies can be used as roughing operations by simply specifying an amount of stock to leave. Below we have listed the most common 2½ Axis toolpath strategies and examples of their use. The Best Practices that we have discussed above will apply to ALL of the 2½ Axis toolpath strategies.

Facing

The Facing toolpath strategy is a method of generating planar toolpaths using Machining Regions as the part geometry limits. The toolpath begins at the top Z value and stops at the bottom Z Depth you specify. The outermost region in facing is treated as a region enclosing a “core” part and thus the system assumes it is safe to approach this region from the OUTSIDE. Such scenarios as shown below. Note that the cutter can be positioned outside these selected regions without violating the part geometry. As a consequence, the system positions the center of the cutter ON the outermost region when cutting. The supported cut patterns are Linear or Island Offset. Clean up passes can be added and stock left around islands automatically as shown on the left image below.

Facing is a planar area clearance operation that supports many different cutting tool types. End Mills and Face Mills are most commonly used. Notice that only the selected Machining Regions are considered allowing sub features such as holes and pockets to be ignored. A cleanup pass at islands can be added automatically.

 

Pocketing

The Pocket toolpath strategy is also a method of generating planar toolpaths using regions as the part geometry limits. The main difference with Pocketing and Facing is that the perimeter of the cutting tool stops at the selected regions. Thus in pocketing the system assumes that you are machining a “cavity” type of part. This means the cutter cannot be positioned outside or on any of these regions. Typical situations where a pocketing toolpath will be suitable are shown below. The toolpath begins at the top Z value and stops at the bottom Z Depth you specify. The supported cut patterns include Offset, Offset Spiral, Linear, Spiral, Radial and High Speed.

In Pocketing, the diameter of the cutting tool stops at the selected regions. In the example on the left the Offset cut pattern is used. On the right we see the characteristic tangential loops of the High Speed cut pattern.

 

Profiling

The Profiling toolpath strategy treats the selected machining regions as the tops of vertical walls spanning from the Z value of the regions down to a specified Z depth. The cutter engagement can be set to Climb, Conventional or Mixed. You can set the Cut Side as well as a Total Cut Width, a Step/Cut distance and more. This strategy supports many Advanced Cut Parameters such as automatic Bridges & Tabs, Cut Arc Fitting, Corner Rounding and Smooth Cut Transitions. A Ramp entry motion is often used with this strategy.

Profiling allows you to cut the perimeter of machining regions. In the example of the left we see a 5 degree ramp entry motion with Arc Fitting (shown in dark blue). On the right we see a finishing Profiling cut around the perimeter of the three inner pockets.

 

Engraving

The Engraving toolpath strategy allows you to select open or closed regions to engrave. In addition to 2D regions, 3D regions can also be chosen. Multiple depths can be specified for better control of the engraving operation. This method is especially suited for engraving text and logos onto part geometry. Unlike the 3 Axis Curve Machining methods, the cutter is not projected to the surfaces below. It merely follows the selected regions.

In the Engraving toolpath strategy the tool tip follows the selected curve regions. You can select from a variety cutting tool types. On the left we see text being engraved onto a part. On the right we see the cutting tool following the selected sketch regions. 

Hole Pocketing

Hole Pocketing can be used to cut larger diameter holes as a milling operation instead of drilling. The hole radius and depth can be specified, along with the number of levels. The Engagement can be specified as a helix with the height and angle or pitch. For machines capable of helix cycles, the output can be a helix cycle. For others, it can be a series of linear moves. Hole Pocketing can be used as a roughing operation by adjusting the Hole Diameter value. You can then follow with the Hole Profiling toolpath for additional roughing and/or finishing of holes.

On the left we see a Hole Pocketing toolpath. The helical engagement is located at the center of the hole where cutting begins. The stepover is then applied until the outer perimeter of the hole is reached. On the right we see the same toolpath with cleanup passes added at each cut level.

Hole Profiling

Hole Profiling can be used to cut circular regions where the interior of the profile needs to be cleared of all material. The hole diameter and depth can be specified. The Engagement can be specified as a helix with the height and pitch angle. Similar to Hole Pocketing, for machines capable of helix cycles, the output can be a helix cycle. For others, it can be a series of linear moves. Hole Profiling often follows a Hole Pocketing toolpath when it is used for additional roughing and/or finishing of holes.

On the left we see a Hole Profiling toolpath. The helical Pitch will determine the Z distance between each 360 degree motion. On the right we can see the radial entry and exit motions clearly.

 

More about MecSoft CAM MILL Modules

The toolpaths shown above were programmed using VisualCAM for SOLIDWORKS. The techniques here are similar for all MecSoft CAM plugins. The MecSoft CAM MILL Module is available in 5 product configurations (Express, Standard, Expert, Professional and Premium). Here are some additional details about each of the available configurations. For the complete features list, visit the products page for each platform at VisualMILL, RhinoCAM-MILL, VisualCAM-MILL for SOLIDWORKS and AlibreCAM-MILL.

  • Express: This is a general purpose program tailored for hobbyists, makers and students. Ideal for getting started with CAM programming. Includes 2 & 3 axis machining methods.
  • Standard: This is a general purpose machining program targeted at the general machinist. This product is ideal for the rapid-prototyping, hobby and educational markets where ease of use is a paramount requirement. Includes 2-1/2 Axis, 3 Axis and Drilling machining methods.
  • Expert: Includes the Standard configuration plus 4 Axis machining strategies, advanced cut material simulation and tool holder collision detection.
  • Professional: Includes the Standard and Expert configuration plus advanced 3 Axis machining strategies, 5 Axis indexed machining, machine tool simulation, graphical toolpath editing and a host of other features. Setup 4: Pocketing & Deep Drill 7
  • Premium: Includes the Standard, Expert and Professional configurations plus 5 Axis simultaneous machining strategies.
November 20, 2017
20 Nov 2017

Part Region Heights in 2-1/2 Axis Machining

I want to take a moment to touch base on another topic related to our previous post Understanding Cut Levels in 2½ Axis Machining. I invite everyone to go back and review this informative post. Today I want to quickly discuss how part region heights are considered in 2½ Axis Machining. When selecting part regions from the Control Geometry tab of the toolpath operation dialog, you are not limited to selecting regions from the same XY plane. In the example shown here, the machining regions selected for the 2½ Axis Pocketing operation are nested (one within the other) and lie on two different XY planes in the Z axis.  

Island Regions

In this example, the inner (island) region is honored at each affected cut level. It is also treated as an island when the Clear Island Tops options is checked from the Cut Levels tab. The heights of the machining regions are honored even if your part only consists of wireframe curve geometry (i.e., if you do not have surfaces or a 3D solid model). That is, the machining regions are treated as the edges of walls & bosses as shown in the example below.

2½ Axis Pocketing with multi-level machining regions selected.

 

Here are the parameters used in this example:

2½ Axis Pocketing Cut Levels tab

Clear Island Tops: OFF

Clear Island Tops: ON


Behavior of Radiused Mills near an Edge

In this next image we have reduced the Rough Depth/Cut value to 0.03 to illustrate how the Z heights AND the XY perimeter of each machining region are honored by the cutting tool. In this case, notice the waterfall effect of the Ball Mill tool as it makes contact with the machining regions at each cut level.  

The cause of this waterfall effect is due to the fact that the contact point of the ball cutter with the machining region or the edge of the wall is the same as the tool end when the height of cut level is the same as the height of the edge. As the cut level height decreases, the contact point moves up on the ball of the cutter pushing the tool end outward until finally the side of the tool starts contacting the region. At this point the waterfall effect ends and the cut levels are offset a constant tool radius distance away from the wall.

Here we see that at each cut level, the Ball Mill tool honors the height of machining region as if it were the edge of a wall producing a waterfall effect.

See Also:

November 13, 2017
13 Nov 2017

The F1 CO2 Racer Body Tutorial

For those of you who are new to MecSoft’s MILL Module plugins (or even if you just want brush up on your CAM skills) we have released a newly updated 130-page step-by-step tutorial on how to program 2-sided (also referred to as flip machining) toolpaths for the F1 CO2 Racer Body shown here.

This tutorial has been written for all of our PC-based CAM platforms (RhinoCAM shown), supports all 5 product configurations and includes the 3D CAD files as well as the completed CAM files! Here is a description of what you will find in this tutorial. A condensed Table of Contents is also provided below.

The F1 CO2 Racer body machined from the Pitsco stock blank (Pitsco #28886).

Bottom Side

The tutorial begins with machining the bottom side of the racer first. You will learn how to define the machine setup including part orientation, machine definition, post, stock, material and work zero definitions. It then goes into details on 3 Axis Horizontal Roughing using Clear Flats and Cut Level controls, 3 Axis Parallel Finishing and 2½ Axis Profiling with multiple cut levels, entry/exit and overlap controls.

You will learn how to create cutting tools including Flat and a Corner Radius Mills. You will learn how to create Information and Setup Sheets as well cut material simulations. The toolpaths shown below are similar for all product configurations.

The Machining Job after completing the bottom side is shown here (similar for all configurations).

 

3 Axis Horizontal Roughing (BOTTOM)

3 Axis Parallel Finishing (BOTTOM)

2½ Axis Profiling (BOTTOM)

Top Side

The tutorial progresses to techniques for machining the top side based on each product configuration. Xpress users will learn how to save toolpath defaults. Standard configuration and higher users will learn how to save and load a knowledge base.

Professional configuration and higher users will learn how to create multiple setups for machining both the bottom and top sides in one Machining Job. The cut material simulations are shown below using the Professional configuration.

The Machining Job after completing the top side is shown here in the Professional (PRO) configuration.

3 Axis Horizontal Roughing (TOP)

3 Axis Parallel Finishing (TOP)

2½ Axis Profiling (TOP)

Table of Contents:

Here is an abbreviated Table of Contents of this tutorial:

About this Guide
Getting Ready
To Machine the BOTTOM Side

  • Define the Machine & Setup (Part Orientation, Machine, Post, Stock, Material, Work Zero)
  • 3 Axis Horizontal Roughing (Create a Tool, Parameters, View & Simulate)
  • 3 Axis Parallel Finishing (Create another Tool, Parameters, View & Simulate)
  • 2 Axis Profiling (Create another Tool, Parameters, View & Simulate)
  • Shop Floor Preparation (Information Sheet, Setup Sheet)
  • Posting G-Code
  • For Standard (STD) & Higher Configuration
    • Save your Knowledge Base
  • For Xpress (XPR) Configuration ONLY
    • Save your Defaults

To Machine the TOP Side

  • For Xpress (XPR) Configuration ONLY
    • Define the Machine & Setup (Machine, Post, Stock, Material, Work Zero)
    • 3 Axis Horizontal Roughing
    • 3 Axis Parallel Finishing
    • 2 Axis Profiling
  • For Standard (STD) & Expert (EXP) Configurations
    • Define the Machine & Setup (Machine, Post, Stock, Material, Work Zero)
    • Load your Knowledge Base
    • Edit your Operations (Edit, View & Simulate)
  • For Professional (PRO) & Higher Configurations
    • Create a New Setup
    • Copy & Paste Operations (Edit, View & Simulate)
  • Shop Floor Preparation (Information Sheet, Setup Sheet)
  • Posting G-Code

Where to go for more Help

How to Download this Tutorial

This tutorial is available as a FREE download to ALL MecSoft AMS (Annual Maintenance Subscription) users. To download this 130-page tutorial+source files, login to your MecSoft VisualSERVE Customer Portal. The download is available in the Knowledge Resources forum in each of the following AMS Product Forums:

More Information

For more information about each of these Mill Module products, including data sheets, videos and other resources we invite you to visit the following product pages:

November 6, 2017
06 Nov 2017

RhinoCAM & Pedalino Bicycles

While most of us (if we’re lucky) get to follow our passion into the workplace, Julie Pedalino from Lenexa Kansas has found a way to combine not one but two of her passions into an exciting new startup company called Pedalino Bicycles. I wanted to give you a quick sneak peek of one of Julie’s cool projects.

_________________________________________________________________________________________________

“We at MecSoft Corporation are both humbled and proud that our RhinoCAM software is helping to enable female machinists and entrepreneurs like Julie to experience the excitement and productivity of CNC technology.

 

We hope you enjoy this inspiring success story!”

_________________________________________________________________________________________________

Shown below are the 4 Axis RhinoCAM toolpaths for one of Julie’s custom-made bicycle frames. The vector line drawing of her own graphic design (shown below) is wrapped onto the outer cylindrical Rhino surface. Then using RhinoCAM’s 4 Axis toolpath strategies (Pocketing, Profiling, Engraving, and Drilling) the design is brought to life on her 4 Axis CNC machining center and Mach3 controller. We’ll be publishing further details of this project and more from Pedalino Bicycles in the coming weeks so stay with us!

(Main Image) RhinoCAM is performing the cut material simulation of a 4 Axis Profiling toolpath. Julie created the vector line drawing of her our graphic design (Top Right) and wrapped it onto the cylindrical surface in Rhino. The 4 Axis CNC machining center and the completed component set are shown on the right.

 

(Left) Julie’s 4 Axis CNC machining center in action cutting RhinoCAM toolpaths from a 4130 Steel sleeve. (Right) we see the completed Bi-laminate Lug with Sleeve.

Julie Pedalino is also a professional artist and graphic designer! Here we see the awesome “Thistle” graphic artwork that Julie created for the for the 4 Axis RhinoCAM project shown above.

 

If you’re a bicycle junkie like me, we invite you to see Julie’s work at pedalinobicycles.com and also on Facebook and Instagram!

October 30, 2017
30 Oct 2017

RhinoCAM & Riverview Hobbies

 

Riverview Hobbies, LLC opened for business in 2010 to produce high quality aftermarket poured-resin products for scale modeling kits, an industry worth upwards of 1.5 billion dollars in the US alone, according to the Hobby Manufacturers Association (HMA).  

Jim Orth, owner/operator of Riverview Hobbies uses Rhino and RhinoCAM to design and program the CNC toolpaths required to machine single and multi-cavity molds for their aftermarket wheel kits. 

Shown below are toolpaths for the Riverview Hobbies RVH121001 Slotted Mag Wheel Kit designed for the 1/12 Tamiya Datsun 240ZG.

We’ll be publishing more details of this project and more from Riverview Hobbies in upcoming weeks so stay with us!

(Main Image) Shown modeled in Rhino, a prototype mold cavity for the Riverview Hobbies RVH121001 Slotted Mag Wheel Kit for the 1/12 Tamiya Datsun 240ZG model kit. On the left we see the RhinoCAM MILL Machining Browser listing toolpaths for the indexed 4 Axis machining job. (Top Right) A production component is shown. (Bottom Right) The 1/12 Tamiya Datsun 240ZG model kit is shown complete with the Riverview Hobbies RVH121001 Slotted Mag Wheel Kit.

For more information about Riverview Hobbies we invite to visit them on the web at  www.riverviewhobbies.com.

October 23, 2017
23 Oct 2017

Best Practices in 3 Axis Machining

3 Axis machining is THE MOST common application for all of MecSoft’s CAM milling plugins. The reason is quite simple. This suite of toolpath strategies can quickly and accurately machine a vast majority of components and tooling required by industry today. In this post we’ll explore some of the Best Practices for machining in 3 Axis using MecSoft CAM.

CAD Geometry

Every 3 Axis machining job begins with a 3D CAD model. Why? Because the surface geometry contained within the 3D model is what drives toolpath calculations. Here are the geometry types supported by 3 Axis toolpaths:

  1. Solids
  2. NURBS Surfaces
  3. Meshes (or STL data)

Solids: Solid models are made up of a collection of surfaces, bound together with no gaps or missing areas, always representing a closed watertight volume. Each of the mating surfaces share edges with other surfaces that make up the solid model. This relationship between surfaces is referred to as the topology of the solid model. Another important characteristic of solids is that there are no intersections or overlaps between the surfaces of the model.

 

An example of a solid model from the SOLIDWORKS Design modeler

 

Surfaces: Surfaces are mathematical entities in a CAD model that can accurately represent both standard geometric objects like planes, cylinders, spheres, and tori, as well as sculpted or free-form geometry. Free-form geometry has a myriad of applications in the design world.

Examples of these are industrial designed forms that make up various consumer items such as car fenders, perfume bottles, computer mice etc. If the host CAD system is a free-form modeler, then you are likely getting NURBS (non-uniform rational basis splines) surfaces by default. Surfaces can be free floating or linked together to form a set of surfaces called poly-surfaces.

An example of NURBS multi-surface model created in the Rhinoceros 5.0 NURBS modeler

Meshes (or STL data): In many application domains, mesh is the data type that is produced and consumed. An example would be in 3D scanning where mesh data is produced as output. While machinable, mesh data is listed third. That’s because a mesh is a polygonal approximation of actual mathematical surface. Mesh geometry can also be data intensive requiring additional computer memory and other resources due to the inefficiency of the data representation. Additionally, the accuracy of machining cannot be improved beyond the accuracy of the approximation of the original model.

Scanned Mesh model in VisualCAD

MecSoft’s 3 Axis machining technology allows you to machine one or more or any combination of these data types. However, the preferred data types are in the order listed due to the reasons mentioned.

CAD File Formats

As the person responsible for machining, you may receive part files that have originated from a variety of different 3D CAD systems. Also, your host CAD system will be able to open or import a variety of these formats. For 3 Axis machining, some file formats are preferred over others. We have listed below, the three most common data types.

  1. Native Files
  2. STEP Files
  3. IGES Files

Native Files: These are the files that are created by the host CAD system that the MecSoft CAM product is running as a plugin.  These are always preferred because you are receiving the native geometry created by the same CAD system. This will result in zero translation errors, which can potentially be encountered if you are importing other file formats. So, for example, if you are using MecSoft’s RhinoCAM-MILL software, then native Rhino files (3dm format) are preferred.

STEP Files: If you receive non-native 3D CAD data, then the next choice are STEP files (*.STP and *.STEP). There are two STEP protocols (AP203 and AP214). Both are acceptable. If the host CAD system is a solid modeler then STEP is the preferred data format. The STEP format has the capability to represent solid models with complete topology (i.e., the relationship between adjacent surfaces) information, while other formats do not.

IGES Files: If the host CAD system is a free-form surface modeler, such as Rhino, then IGES would be the preferred data format. The IGES entity type 144 will output trimmed surfaces that are free floating and do not include topology information.

Best Practices:

  1. Try to use the native format files of the CAD product that you are running MecSoft CAM in.
  2. If the sending system is a solid modeler ask for STEP files.
  3. If the sending system is a free-form modeler ask for IGES files.
  4. If you are unsure, ask for both STEP and IGES files.
  5. If possible try to avoid mesh data files such as STL if more accurate representations can be obtained.
  6. For 3 Axis machining, avoid any drawing file formats such as DWG and DXF. You NEED surfaces, NOT 2D drawings and NOT 3D wireframe files.

Effect of Machining Tolerances

Tolerances play a vital role in machining accuracy. There are tolerances from different sources that can come into play to affect the accuracy of your machined part. There are Machine Tool limitations that require the CAM system to make calculations which are affected by tolerances of varying sources. There is the geometry tolerance of the host CAD system. There is a global tolerance associated with each toolpath. There are also arc fitting tolerances and post definition tolerances! You get the idea.

It is best that you understand each of your tolerances and adjust them according to YOUR machining accuracy requirements. We strongly recommend that you read our blog post How to Increase Toolpath Accuracy so that you have a much broader understanding of how tolerances play a role in CAM.

Best Practices:

Below are 10 things to remember regarding tolerances in random order (except for #1):

  1. Check ALL of your tolerance settings.
  2. Internally to MecSoft CAM, all computations are performed in double precision or in an accuracy up to fourteen decimal places!
  3. For designing make sure your geometry tolerance is set to at least six (6) places of accuracy.
  4. For 3 Axis toolpaths, a Global Tolerance is used to control the acceptable deviation of the toolpath from the designed geometry. Adjust this tolerance as required.
  5. For the Arc Fitting Tolerance, two times the toolpaths global tolerance is recommended to allow for the optimal fitting of arcs. If the machined part MUST be within 0.001 of the 3D part, set the Arc Fitting Tolerance to 0.001 and the toolpaths Global Tolerance to 0.0005.
  6. Use the Compare command from the Simulate tab to perform Part/Stock calculations. This will display the resulting tolerance deviation of your machined part!
  7. Check your post processor definition parameters to make sure you are outputting g-code with the required number of decimal places needed to achieve the precision required.
  8. Make sure your CNC controller is set to read and display the decimal place precision required.
  9. Remember that tighter tolerances will result in longer toolpath computation times as well as the creation of longer g-code programs.
  10. If you require tight tolerances in multiple toolpaths from complex solid/surface geometry, go to the Machining section of your CAM Preferences, and check the box to Always generate toolpaths in multiple threads. This will speed up processing times if you have a multi-core processor.

The Role of Stock to Leave

Being a subtractive manufacturing process, CNC machining is all about removing stock. The less stock you have to remove, the less time the machining job will require. Your control geometry can be used to contain the toolpath and limit the amount of stock removal. See Containing your Toolpaths below for more information.

Also, each toolpath strategy has a stock value that you can adjust to your advantage. It can be a positive or a negative value. It determines how much stock to leave or remove in relation to the part surface. A positive stock value leaves material above the surfaces. A negative stock value will remove material below the surfaces. Typically, you would leave successive amounts of material, by defining different values of stock, on the part geometry in roughing operations and will cut to the exact part geometry in the final finish operations.

Best Practices:

  1. Analyze your part geometry and adjust your stock values to minimize the need for remachining.
  2. Finishing operations can be used for roughing or pre-finishing simply by adjusting the amount of stock to leave on the part.
  3. If your CAD geometry does not account for fit, you can use positive and negative stock on mating parts to achieve the fit desired during assembly (press fit, slip fit, etc.).
  4. For finishing operations, the stock value is typically set to zero so as to produce the desired part geometry.

How to Control Surface Finish

Before implementing your machining strategy, determine the surface finish that your part requires. The tolerances you use, part’s form & function, stock material properties, the tools that you use, the cutting feeds that are employed and the machine tool capabilities will all have varying degrees of effect on the surface finish. You might have to do some experimentation with different cutting tolerances, machining strategies and methods to determine when to use what method to yield the best surface finish you desire.

Best Practices:

  1. Use machining regions that contain your toolpaths to flow with the geometry of the part. See the Containing your Toolpaths section below.
  2. Use different cut patterns and/or direction of cuts in areas with a specific geometric feature and remachine to obtain better surface finishes. Use this in conjunction with containment regions to make the machining more efficient.
  3. Combine your toolpath strategies to achieve a better surface finish. You can read more about this under the Operation Types and their Typical Uses section below.


Using successively smaller tool sizes to remachine a critical area is another approach to get better surface finish. The idea here is to use the large cutter(s) to remove most of the material and the smaller cutter(s) to perform light cuts and also to cut in areas where the larger cutters could not cut due to geometrical constraints in the part.

General Machining Strategy

After geometry, file formats and tolerances, the next process is to evaluate your general machining strategy. This can largely depend on your part size and geometry. Will the part fit on your CNC machine? If not, can you machine it in sections? Can you machine all of the required features from one side or will the part need to be flipped over for secondary setup and machining? Once these general questions are answered, you can move on to specific toolpath strategies. Here is the general machining strategy you can apply to all parts.

Best Practices:

  1. Look at how much stock needs to be removed. If you are cutting flat sheets and simple cutouts, then 3 Axis machining may not be required or even desired. Look at 2½ Axis Machining instead.
  2. If your part has ANY tapered walls then you know that 3 Axis toolpaths ARE required.
  3. For 3 Axis machining, the typical approach is roughing first. Then pre-finishing and/or finishing. After this you may need some detail cleanup and possibly remachining. See 3 Axis Toolpath Strategies below for specific toolpath strategies.

Operation Types and their Typical Uses

Your 3D part geometry and required surface finish both play a key role in determining what toolpath strategies to use for any given part. The goal in 3 Axis machining is to calculate a path on and along the surfaces of the part for the cutting tool to follow. In general, 3 Axis toolpaths are projected onto the underlying surfaces. We will review each 3 Axis toolpath strategy available in the Standard (STD) configuration and suggest how they can be best utilized.

Horizontal Roughing

This is the bulk material removal strategy. It removes material in levels from the raw stock model. The tool starts at the top of the stock model and removes material without changing its Z position and only moving in the XY plane. Once this level is completed, the tool moves to the next lower Z level and removes material in this XY plane. This procedure is repeated until the bottom most Z level is reached. The spacing between cut levels can be specified. You can also contain the toolpath to only cut between a top and bottom cut level.

Best Practices:

  1. If you want to clear horizontal sections of the part that are located between cut levels, just check the Clear Flats box from the Cut Levels tab.
  2. Horizontal Roughing supports five different tool types. Use them according to your needs.
  3. You can specify a start point to begin cutting. Look at the Start Points tab of the Control Geometry tab of the dialog. This is used when machining hard materials and also when you have tools that cannot plunge into material. A pre-drilled hole can be made at the start point to prevent the milling tool from plunging into material.
  4. Horizontal Roughing allows separate cut parameter controls for Cavity/Pocket and Core/Facing regions that are encountered during machining. Cavity/Pocket areas are fully enclosed areas needing the tool to plunge into the material for machining. Core/Facing regions have openings and the tool can come from outside stock and thereby prevent plunging into material.
  5. Be sure to review and understand every option on the Cut Parameters tab.

Part Examples:

The illustrations below show how Horizontal Roughing can be effectively used to remove stock material in targeted areas.

   
The part is shown on the left. The stock model is added on the right.
   

In the image on the left, no machining regions are selected, allowing the tool to clear all accessible stock. In the right image, the bottom outer perimeter of the part is selected limiting the tool to within that area only.

In this image the lower perimeter and the upper perimeter are both selected, limiting the tool to cut only between the two regions. All of the above conditions (and more) are available using the 3 Axis Horizontal Roughing toolpath strategy.

Parallel Finishing

This is one of the most commonly used strategies for finishing. The cutter is restricted to follow the contours of the part in the Z direction while being locked to a series of parallel vertical planes. The orientation of these vertical planes (referred to as the Angle of Cuts) can be defined and is measured from the X axis. The tools typically employed in this operation are Ball and Corner Radius mills.

This strategy is best suited for parts that are more horizontal than vertical. Because the tool is projected vertically down, as the part geometry become more vertical, the toolpaths become further apart in the vertical axis leaving more stock material than usual.


Best Practices
:

  1. By default, the center of the tool will stop ON the machining regions selected from the Containment Regions tab of the Control Geometry tab of the dialog.
  2. This strategy is often used in pairs to maximize coverage and to achieve a better surface finish. The only difference being the Angle of Cuts. Typically, these are set 90 degrees apart. Be sure to review and understand every option on the Cut Parameters tab.
  3. If you wish to overcut the part, a negative stock to leave value can be used. However, note that the value of this negative stock cannot be greater than the radius of the tool.
  4. This strategy can also be used for roughing by enabling the option Insert multiple step-down Z cuts from the Z Containment tab of the dialog.
  5. You can Ignore Holes in your part while using this strategy. This is located in the Cutting Area Control section of the Cut Parameters tab of the dialog.
  6. If your part geometry has a lot fine detail, try using a Taper mill with this strategy. This cutter type provides the smaller ball mill radius at the tip combined with a taper angle on the sides. Have a look at the example in our blog post The Trinket Box by Bernie Solo. Lid – Part 1 of 2.

Part Examples:

Here are some examples of using the Parallel Finishing strategy.

The Parallel Finishing toolpath follows the part in the Z axis calculating the contact points of the tool and the surfaces. At the same time the center of the tool stops at the selected machining regions (highlighted in orange) in X and Y. Notice that these regions do not have to lie on the surfaces being machined. These two toolpaths are programmed with Cut Angle set to zero and ninety degrees to maximum material removal and best surface finish.
 
In these two examples, the Parallel Finishing toolpath is contained to the perimeter of the cavity only, again with Cut Angle set to zero and ninety degrees to maximum material removal and best surface finish.

Horizontal Finishing

In this strategy the cutter finishes in constant Z planes and is suitable for parts with steep walls where the upper radius and sides of the tool are used. The tool types commonly used in this method are Ball and Corner Radius mills.

This strategy is best suited for parts that are more vertical than horizontal. Because the toolpath is computed as slices of the part geometry in horizontal planes, in areas where the part geometry is close to flat, toolpaths become further apart in the horizontal plane leaving more uncut material than in other areas. This will necessitate the use of additional toolpaths or the optimized machining setting to remove this uncut material.


Best Practices
:

  1. Be sure to review and understand every option on the Cut Parameters tab.
  2. If your part has areas that are more horizontal than vertical, you can optimize XY machining between levels. This can be enabled from the Optimized Machining tab of the dialog. Refer to the part examples below.
  3. Similar to Horizontal Roughing, you can also Clear Flats automatically during this strategy. The option is in the same location on the Cut Levels tab of the dialog.

Part Examples:

Notice that the core and cavity of this mold example has steep walls. The toolpaths on the part are calculated using a set of parallel Z planes. The distance between these planes is controlled by the Stepdown Control section of the Cut Levels tab of the dialog.

   
(Top Left) Notice in this image that no toolpaths are calculated for surfaces that are horizontal. You can use this to your advantage if you plan on cutting these areas separately. (Top Right) You can also add toolpaths to these horizontal areas automatically using the Optimized Machining tab of the dialog. You can independently control the XY Stepover distance and the Entry/Exit motions for these areas.
Here we see the cavity side of the mold. (Top Left) No Z level containment is specified. Toolpaths are calculated for all part surfaces the tool can access. (Top Right) From the Cut Levels tab of the dialog you can contain the Top and Bottom Z levels of the toolpath.

Spiral Machining

This strategy is best used as a finishing operation for regions that have circular characteristics. Spiral cuts are generated inside an enclosed machining region, extending from a center point. It requires machining regions to be selected from the Control Geometry tab. The start point of the cuts can be set to start from outside or inside. You can specify the center point or allow the system to calculate the optimum center point.

This strategy is best suited for parts that are more horizontal than vertical. Small motions of the tool in the horizontal plane when the tool is travelling along a vertical feature of the part geometry, can cause large changes in the vertical plane, resulting in the tool going up and down. This can result in bad surface finishes. So, care must be used when using this strategy with parts with vertical areas.


Best Practices
:

  1. Spiral Machining & Radial Machining are often used together to maximize coverage and to achieve a better surface finish. That’s because the cut direction of the Radial toolpath will always bisect the cut direction of the Spiral toolpath when used on the same machining regions.
  2. This strategy can be used for roughing by enabling the option Insert multiple step-down Z cuts from the Z Containment tab of the dialog.
  3. This strategy can be just as effective on machining regions that are only circular in nature. The Spiral Parameters section of the Cut Parameters tab can help you control the position and scope of this toolpath. Be sure to review and understand every option on the Cut Parameters tab.

Part Examples:

We have used the same part example as the Radial Machining strategy above. Notice that the part’s feature is circular in nature. Also notice that the machining region selected does not have to be circular. The spiral toolpath will be calculated for any closed region.

 

   
(Top Left) The spiral toolpath is calculated for a circular machining region.  (Top Right) The same toolpath is calculated with Minimum Diameter specified.
(Top Left) The spiral toolpath is calculated for a circular machining region with Minimum Diameter specified. (Top Right) The same toolpath is calculated using the irregular machining region around the perimeter of the feature.

Radial Machining

Similar to the Spiral Machining strategy, this strategy is best used as a finishing operation for regions that have circular characteristics. Linear cuts are generated inside an enclosed machining region, extending from a center point. It requires machining regions to be selected from the Control Geometry tab. The start point of the cuts can be set to start from outside or inside. You can specify the center point or allow the system to calculate the optimum center point.

This strategy can be used for parts that are both vertical as well as horizontal. This method works well in areas where Spiral Machining performs poorly. However due to the nature of the cut pattern, over cutting can take place near the center of the radial pattern.


Best Practices
:

  1. Spiral Machining & Radial Machining are often used together to maximize coverage and to achieve a better surface finish. That’s because the cut direction of the Radial toolpath will always bisect the cut direction of the Spiral toolpath when used on the same machining regions.
  2. This strategy can be used for roughing by enabling the option Insert multiple step-down Z cuts from the Z Containment tab of the dialog.
  3. This strategy can be just as effective on machining regions that are only circular in nature. The Radial Parameters section of the Cut Parameters tab can help you control the position and scope of this toolpath. Be sure to review and understand every option on the Cut Parameters tab.

Part Examples:

Notice that we used the same part examples as in Spiral Machining above.  In these examples the part feature is radial in nature. Also, the machining region selected does not have to be radial. The radial toolpath will be calculated for any closed region.

(Top Left) The radial toolpath is calculated for a circular machining region. (Top Right) A Minimum Diameter is specified that limits the center of the feature from being machined.
   
(Top Left) The radial toolpath is calculated for a circular machining region, Notice the overcutting near the center.  (Top Right) The same toolpath is calculated using the same circular region but with a Minimum Diameter specified.  

Containing your Toolpaths

The dialog of each toolpath strategy in MecSoft CAM includes a Control Geometry tab. In 3 Axis machining, this tab is used to define machining regions that contain the toolpath so that it cuts only in the areas you want to cut. By understanding how to contain your toolpaths you can minimize machining time and achieve a better surface finish.

Best Practices:

  1. Select machining regions that allow the cutter to move with the flow of your part.
  2. Use machining regions to minimize the amount of material to be removed during roughing. A common strategy is to creating a silhouette curve around the perimeter of your part. Then offset that curve by 1.5 times the diameter of the roughing tool. Then use that resulting curve as your machining region. This allows room for the tool to reach the part surfaces while containing it to a minimum area.
  3. We have some excellent blog posts that discuss the effective use of machining regions:
    The Anatomy of a RhinoCAM Part
    2-Sided (Flip) Machining Explored
    Bridges & Tabs Explored
    Techniques for Machining Ring Jewelry
    What is Surface Feature Machining?

Part Examples:

The core block part shown below is a good example of how machining regions can be used to contain your toolpaths in 3 Axis machining.  In these toolpath examples we have enlarged the stepover distances so that you can see the toolpath clearly.

   
The image on the left shows the 3 Axis Part and on the right we see the Horizontal Roughing strategy with no machining regions selected as containment. The tool removes all material from the stock that it can reach.
   
The image on the left shows an initial Horizontal Finishing strategy using the outer perimeter of the rectangular base of the core block for containment. Notice that only the surfaces that are NOT horizontal are machined. The image on the right shows the use of Parallel Finishing in a contained area. With the Angle of Cuts set to zero, the tool follows the radius of the part.
   
Here we see the use of the Radial Machining and Spiral Machining strategies to finish the circular feature on the top of the part. The circle at the base of the feature is used for containment.

Here we see the use of the Radial Machining strategy that is contained by the outer perimeter of the set of surfaces that define an irregular but circular feature on the part.

 

More about the MecSoft CAM MILL Module

The toolpaths shown above were programmed using VisualCAM for SOLIDWORKS. The techniques here are similar for all MecSoft CAM plugins. The MecSoft CAM MILL Module is available in 5 product configurations (Express, Standard, Expert, Professional and Premium). Here are some additional details about each of the available configurations. For the complete features list, visit the products page for each platform at VisualMILL, RhinoCAM-MILL, VisualCAM-MILL for SOLIDWORKS and AlibreCAM-MILL.

  • Express: This is a general-purpose program tailored for hobbyists, makers and students. Ideal for getting started with CAM programming. Includes 2 & 3 axis machining methods.
  • Standard: This is a general-purpose machining program targeted at the general machinist. This product is ideal for the rapid-prototyping, hobby and educational markets where ease of use is a paramount requirement. Includes 2-1/2 Axis, 3 Axis and Drilling machining methods.
  • Expert: Includes the Standard configuration plus 4 Axis machining strategies, advanced cut material simulation and tool holder collision detection.
  • Professional: Includes the Standard and Expert configuration plus advanced 3 Axis machining strategies, 5 Axis indexed machining, machine tool simulation, graphical toolpath editing and a host of other features. Setup 4: Pocketing & Deep Drill 7
  • Premium: Includes the Standard, Expert and Professional configurations plus 5 Axis simultaneous machining strategies.0

 

October 16, 2017
16 Oct 2017

Understanding Climb vs. Conventional Milling

One of the basic concepts to understand in any milling operation is Cut Direction. It can be characterized by how the flutes of the cutting tool engage the stock material and form the chip that is removed during cutting. In many of MecSoft CAM’s 2½ & 3 Axis toolpath strategies you will see that Cut Direction is defined by selecting one of three options, Climb, Conventional or Mixed. Let’s take a look at the characteristics of each option.

Climb Milling

Consider each chip being removed as a wedge of material that has a wide end and a narrow end. In Climb milling (also referred to as a down cut) the relationship between Spindle direction and Cut Feed direction combine in such a manner that the wide end of the chip is removed first and the narrow end removed last. This means when the cutter tooth first comes in contact with the workpiece it removes the maximum amount of material (chip width being maximum). As the cut progresses, the amount of material being removed decreases and just before the flute loses contact with the workpiece the chip width is zero. This produces a climbing effect of the cutting tool on the workpiece material as shown in this illustration. The linear distance of the wide end of the chip is referred to as the Feed per Tooth.

Because chips are discarded behind the cutter, the chances of the cutter re-cutting the discarded material is reduced. Climb milling also reduces wear on the cutting tool because rubbing (i.e., contact without cutting) on the workpiece is reduced. Also, the maximum force on the workpiece occurs when the cutter is taking the biggest bite out of the workpiece. The force at this point is directed straight down on the workpiece. This keeps the workpiece more stable with less stringent work fixturing required. However, due to the sudden increase in the force, active management of tool backlash is necessary.

Climb milling is the preferred method of cutting since it results in a better surface finish. However due to the larger forces encountered at the beginning of each cut, machines and spindles have to be more rigid.

Conventional Milling

In Conventional milling (referred to as an up cut) the narrow end of the chip at the bottom of the cut is removed first and the wide end removed last. This produces the up cutting effect of the cutting tool on the stock material as shown in this illustration. The Feed per Tooth is not fully realized until the end of the chip removal.

Because chips are discarded upward in front of the cutter, re-cutting of the chips can occur, which can result in a rougher surface finish. Conventional milling can also increase wear on the cutting tool because of increase of rubbing between the tool and the workpiece at the start of the cut where the cutter is not removing any material.

The maximum force on the workpiece occurs when the cutter is taking the biggest bite and then losing contact with the workpiece. At this point the force on the workpiece is directed upwards. This requires the need for more stringent work fixturing than climb milling. However, the cutting forces go from zero to maximum without any sudden increases resulting in less tool deflection.

Even though climb milling is preferred, there are times when conventional milling is used such as when machining materials which have rough or hardened surface finishes. Climb milling on these materials can result in undue forces when the cutter teeth make first contact with the workpiece material.

Mixed (Climb/Conventional) Milling

The Mixed option simply means that the CAM software uses a combination of the two milling directions within the same toolpath. This option is typically used in finishing cuts when very small amounts of material are being removed. A Mixed cut direction can reduce tool travel and the number of retracts and transfer motions, thus saving machining time.

Let’s Review:

  1. Consider each chip being removed as a wedge of workpiece material.
  2. The distance at the widest end of the chip is the Feed per Tooth.
Climb Milling (Down Cut):
  1. Less re-cutting of chips, higher quality surface finish.
  2. Less wear on the cutting tool (tool life is extended).
  3. More tool deflection encountered but less fixturing needed (cutting force is directed onto the workpiece).
  4. Machines and spindles need to be more rigid.
Conventional Milling (Up Cut):
  1. More re-cutting of chips, lower quality surface finish.
  2. More wear on the cutting tool (tool life is reduced).
  3. Less tool deflection encountered but more fixturing is needed (cutting force is directed away from the workpiece).
  4. Machines and spindles can be less rigid.
Mixed (Climb/Conventional) Milling:
  1. A combination of both methods is used within the same toolpath.
  2. Typically used in finishing toolpaths.
  3. Can reduce tool travel and machining time.
October 9, 2017
09 Oct 2017

Understanding Cut Levels in 2½ Axis Machining

In 2½ Axis machining, machining is performed in multiple Z levels, where the cutter moves in both the X and Y axes while the Z depth is fixed at each of these Z levels. This fixed Z depth is maintained until all of the stock material is cleared for that level. The cutter then moves down in Z and begins clearing the next XY level.

One of the benefits to 2½ Axis machining is that you do not need a 3D model. A 2D drawing works just fine. An obvious limitation is that you can only machine prismatic parts, where all of the side walls are vertical. For many applications however, this limitation is not only acceptable but absolutely required.

As you may imagine, an understanding of how cut levels are controlled for 2½ Axis machining in MecSoft’s CAM plugins is essential. In this post we will discuss the toolpath operations that share the majority of the same Cut Levels tab options. These include 2½ Axis Facing, Pocketing, Profiling, V-Carve Roughing and Slotting.

If you look at the upper image in the dialog you will see that the Location of Cut Geometry and Cut Depth Control param eters are illustrated. To help you understand these controls we will use the pocket examples shown below.

Location of Cut Geometry

Cut Geometry refers to the Part Regions in the Control Geometry tab that you will select to define the cut pattern. These are typically 2D curve geometry and if you have a 3D model might include edge curves or flat area selections. The three options in the dialog At Top, At Bottom and Pick Top are best explained for any instance by simply asking yourself this basic question:

“Where is my cut drive geometry located in relation to the starting Z level?”

Typical 2½ Axis Pocket with Location of Cut Geometry At Top

Typical 2½ Axis Pocket with Location of Cut Geometry At Bottom

In the pockets shown here you can clearly see that the selected cut geometry is located at the bottom of the pocket, so At Bottom is selected from the dialog. This means that the Cut Depth Controls in the dialog are measured from this location upward in Z. In a different part model, it might be convenient to select the curves located at the top edge of the pocket. In such cases the At Top parameter would need to be selected. Let’s continue this example and have a look at the other parameters in the dialog. We will discuss the Pick Top option further down in this post.

Cut Depth Control

The Cut Depth Control parameters allow you precise control of the cutter’s Z depth at each cut level in the pocket. For example, Total Cut Depth will be total amount of Z travel you want when performing the machining. This is an absolute value in the dialog (i.e., no positive or negative). You can enter this depth value directly or use the Pick button to select two points from your 3D part model and the depth is calculated and added to the dialog for you.

Rough and Finish Cut Depths

Rough & Finish Cut Depth Controls

If desired, you can divide this total cut depth into a Rough Depth and a Finish Depth by entering the values or using the sliders provided. You can go even further by entering the depth per cut for each of the rough and finish depths. In our example here, we have the Total Cut Depth set to 1.25. This depth is divided into a Rough Depth of 1 and a Finish Depth of 0.25. The Rough Depth/Cut is set to 0.25 and the Finish Depth/Cut is set to 0.05. You can see in the illustration above that these values divide the rough depth into 4 levels (each 0.25) and the finish depth is divided into 5 levels (each 0.05). Keep reading and we will also discuss the Clear Island Tops option and the Use 3D Model to Detect Depth option.

Using the Pick Top Option

There may be situations when the cut geometry available for selection is neither located at the top nor at the bottom of your desired pocket. For example, you are machining from a 2D drawing and the geometry of the drawing is aligned with the bottom of your stock. You may want the depth of the pocket to be measured from the top of the stock or you may want to start cutting slightly above the stock. Have a look at the illustration and dialog below.

2½ Axis Pocketing from 2D Geometry using Pick Top

This cross-section diagram illustrates how the Pick Top option works. In this example there is no 3D model. The Control Geometry is a 2D drawing located on the XY plane at Z0 (zero). You are looking at the resulting stock after the pocket is cut. Notice that the Stock Height and the Pick Top value are the same (0.5).

2½ Axis Pocketing Cut Depth Control using Pick Top

When we defined the stock, we set the H dimension in the Box Stock dialog (shown on the left) to 0.5. By setting Pick Top to 0.5, the cut starts at the top of the stock. You can also think of this as moving the cut geometry up to this Z location. The Total Cut Depth is set to 0.25 and the Rough Depth/Cut is set to 0.05. This produces the 5 cut levels that you see in the cross-section above. Let’s take this one step further and say for example that the bottom of your stock is nice and flat but the top is not. You could then set the Pick Top value to begin the cut slightly above the stock, say at 0.6. As you can see the Cut Levels tab provides precise control of your cutting.

Clear Island Tops

There may be situations when there are one or more islands located within the pocket. Island refers to material that protrudes up from the floor of the pocket and whose sides do not touch the sides of the pocket. When you check the option to Clear Island Tops, an additional cut level is located at the top of the island. If there are more than one and they are at different heights an additional cut level is added at each island top. It is important to note that if you have selected curves as your cut geometry, the heights of the curves will be honored by the system. This feature allows you to select curves to define island tops in multiple depths as in the model shown here.

Using the Clear Island Tops Option

 Use 3D Model to Detect Depth

As the name of this option implies, checking this box will allow the CAM system to determine the depth of the pocket for you based on your 3D part model. You see that with this option checked, the Total Cut Depth and Rough Depth fields in the dialog become inactive. The Finish Depth is automatically measured from the bottom of the pocket and both Depth/Cut controls are still available. Note that a 3D part model is required to use this option.

This option can be very useful when loading a knowledge base for machining automation with various 3D parts. If this option is set in the Knowledge Base operation, there is no need for the user to manually specify the total cut depth depending on the loaded part. It will be automatically computed from the current 3D model.

Cut Controls with Use 3D Model to Detect Depth Enabled

Cut Depth Controls when Machining a Feature

When MecSoft CAM is machining a detected feature, such as the pocket in the above example, the Cut Depth Controls on the Cut Levels tab are adjusted to match the feature. For example, the minimum depth required to machine the feature is displayed in the dialog and cannot be changed. You can however, adjust the Rough Depth/Cut, and specify a Total Finish Depth and a Finish Depth/Cut If desired. The dialog below shows the values that will cut the same pocket shown in the example above.

Cut Depth Control when machining a feature

 The controls discussed in this post apply to the following 2½ Axis Milling toolpath strategies in VisualCAD/CAM (VisualMILL), RhinoCAM-MILL, VisualCAM-MILL for SOLIDWORKS and AlibreCAM-MILL:

  • 2½ Axis Facing
  • 2½ Axis Pocketing
  • 2½ Axis Profiling
  • 2½ Axis Slotting
  • 2½ Axis V-Carve Roughing