Archive for year: 2021

September 23, 2021
23 Sep 2021

Strategy for a Radial, Ramped, Counterbored Keyway Slot

The content for this article comes to us courtesy of David St. Angelo, CNC Programmer & Operator with Jim Thompson Marine Carpentry (JTMC), located at 1 Washington Street, Newport, RI the Newport Shipyard’s carpentry shop, specializing in Yacht Carpentry, Finishing, Furnishings and more.

Watch the companion video here!

Blog Contents:

The Part

Note: All dimensions mentioned in this article are in millimeters (mm). This part is referred to as Viasat. It is used as a mounting bracket for a large satellite receiver on the top of a 90 foot catamaran. The CAD geometry for this project is a 375.0 diameter x 25.00 thick ring of T10 steel (very hard). Please refer to the illustrations below for reference. The ring contains 4 keyway slots that are 22.00 wide, 58.730 long and are positioned along a 142.42 center-line radius. So the length of each keyway slot is on a radius. Each keyway also contains a stepped counterbore. The full 22.00 wide keyway drops down to 10.00 before narrowing to 11.96 wide. What makes this keyway feature very unique is that the base of the counterbore ramps downward 5 degrees on each side. You can refer to the elevation images below for more details.

 

The ring plate is 375.0 in diameter and 25.00 thick. The ramped keyway is located in each 90 degree quadrant. Each keyway is 22.00 wide x 58.73 long and is centered along a 142.42 diameter. 

 

What makes this keyway feature very unique is that the base of the counterbore ramps downward 5 degrees on each side. The elevation view below shows a cross section of the ramp clearly. The length of the ramp is approximately 16.00 long. The ramp also occurs on both sides of the keyway.

 

(Left) A cross-section view of the 5 degree ramped counterbore portion of the keyway. (Right) An isometric view of the keyway showing the portion of the counterbore that is ramped downward 5 degrees.

 

Additional CAD Geometry

In many machining strategies you will want to add reference geometry that will help guide your toolpaths. In this example we are adding the two curves shown in the illustration here labeled Inner Curve and Outer Curve. We created these two curves by (1) creating curves that are offset inward from the base of the counterbore (this is the 10.00 depth dimension shown above). These curves define the 5 degree ramp angle. (2) We then joined and trimmed these new curves into just two curves, one inner curve and one outer curve. After that (3) we added another half circle curve of radius 3.905 positioned on the outer curve at the end closest to the thru hole. This half circle curve is labeled “Radius for Engraving” in the illustration. We have also added a geometry point located at the top of the 22.00 thru hole. This point is labeled Start Point for Roughing in the illustration. As described, this point will be used as the cut start point for a 3 Axis Roughing operation. 

 

Let’s review:

  1. We created curves that are offset from the base of the keyway inward by a distance of 3.905 which is the radius of the flat end mill tool we plan to use.
  2. We then merged and trimmed these curves to form just two curves, one inner curve and one outer curve.
  3. We also added a new curve that is a half circle and located it at the end of the outer curve closest to the thru hole.
  4. These curves will drive the center tip of the tool during a 2½ Axis Engraving operation.
Add Machining Regions

In this step we will create 4 pre-defined machining regions. MecSoft CAM allows you to create machining regions and save them for use with toolpath operations. In this example we will predefine 4 machining regions. We will use these regions to drive our cutting tool during a 2½ Axis Engraving toolpath operation. See Finishing Operations below for more about how these predefined regions are used. Also refer to the Optional Methods section below. You will also find suggestions on alternate methods to achieve the same goal.

When we are finished creating the predefined regions, the Regions tab of the Machining Objects Browser will look like the image below. We see that there is one Machining Region Set: Radial Slot that contains 4 regions below it. These 4 regions are named Slot Top, Slot Bottom, Slot Ramp Outer and Slot Ramp Inner. 

 

The Region tab (identical for all MecSoft CAM plugins)

 

The toolbar on the Regions tab contains the icons and commands you need to create the region set and the four regions. These are the first two icons on the left side of the toolbar. The first being the Create Machining Region Set command. Selecting it adds a new set with nothing under it. Then when you pick the Select Curves icon, you are prompted to select curves. So we selected the top edges of the keyway slot and pressed enter. A region named “Curve Region #” is added under the region set. If you create the region first, the region set is added automatically. We then renamed this region as Slot Top. 

Slot Top

Slot Bottom 

Slot Ramp Outer

Slot Ramp Inner

We repeated this procedure to create a region named Slot Bottom. We then created the two regions named Slot Ramp Outer and Slot Ramp Inner. You can also select all of the 4 curves at one time and add each to the set and then rename them. Now when you select each region from the Regions tab you see that they highlight green on the part. The illustrations above show you what each region looks like.

The Stock & Setup

The stock definition for this project is a Part Bound Cylinder Stock. It is referred to as Part Cylinder Stock on the Stock menu on the Program tab. This stock definition computes the size of your part and then allows you to add an offset value to both the Radial and the Axial dimensions. You can also set the axis of the cylinder and the Axial Offset Direction. In our case we selected the Z axis, set the Radial Offset (r) to 5, the Axial Offset (a) to zero. Since we set the Axial Offset (a) to zero, we need not bother with setting the Axial Offset Direction as it will be ignored. Also, to make sure only the 3D solid was calculated, we checked the box to Ignore Wireframe Geometry in Bounds Computation. The stock and stock dialog are shown below.

 

Here we see the Part Bounding Cylinder Stock dialog on the left and the graphic representation of the stock overlaid onto the part model. You can see that 5mm is added to the diameter of the part.

 

Sequence of Operations

The Machining Job and Setup 1 shown below includes two Drilling operations, one 3 Axis operation and three 2½ Axis operations. Note that the 2½ Axis Engraving operation cuts the 5 degree ramp and is the next to the last operation in the Machining Job. The last operation is the Polar Instance that will cut the remaining 3 keyway slots automatically. Also refer to the Optional Methods section below. You will find suggestions on alternate methods in this operational sequence.

The Machining Job tree shows all machining operations (MOps) in Setup 1. The first six MOps will cut the first Keyway slot. The last operation will cut the remaining 3 keyway slots.

Here we see a cut material simulation of the first six operations under Setup 1 to cut the first keyway slot. Note that the last 2½ Axis Engraving operation is the finishing cut for the 5 degree ramp.

Drilling Operations

We have used Drilling as the first two operations. These will spot drill (referred to as a Center Drill) a 6mm x 1mm deep hole followed by a Deep Drill to drill a 14mm dia hole through the part at 5mm step increments. The Add Tooltip to Drill Depth option is checked to make sure the drill passes completely through the part. These two drilling operations are illustrated at (A-1 & A-2) and (B1 & B2) in the table below. The toolpath is shown on the left and the resulting cut material simulation is shown on the right. Both drilling operations are located at the Point geometry that we added at the top of the 22 diameter through hole on the keyway. 

(A-1) Here we see the first drill operation toolpath. This will spot drill (referred to as a Center Drill) a 6mm x 1mm deep hole,

(A-2) Here we see the cut material simulation showing the in-process stock remaining after the spot drill is completed.

(B-1)Here we see the Deep Drill operation toolpath. It cuts a thru hole 14mm in diameter.

(B-2) Here we see the cut material simulation showing the in-process stock remaining after the Deep Drill is completed.

 

Roughing Operations

The next two operations in the Machining Job are considered roughing operations. They are a 3 Axis Horizontal Roughing and a 2½ Axis Pocketing operation. The 3 Axis Horizontal Roughing is used to rough cut the upper counterbore level of the keyway. For the Control Geometry tab we are picking the Select Predefined Regions button to display the Select Predefined Region(s) dialog shown here. Selecting Slot Top and picking OK, assigns that region to this operation.

For the Cut Parameters tab, Stock is set to 0.5, an Offset cut pattern, Mixed cut direction and a 25% (of the tool diameter) stepover. On the Cut Levels tab the Stepdown is set to 2 levels and the Bottom (B) under Cut Levels is set to -10.84 which is the bottom of the 5 degree ramp. The engage and retract are set to helix motions. This toolpath and resulting cut material is shown at (C-1 & C-2) below. It should be noted here that David wants to use the same cutter for all milling operations.

(C-1) Here we see the 3 Axis Horizontal Roughing operation toolpath. It rough cuts to the counterbore level.

(C-2) Here we see the resulting cut material simulation showing the in-process stock remaining after the 3 Axis Horizontal Roughing operation is completed.

The next operation in the Machining Job is 2½ Axis Pocketing. You can see the toolpath and the cut material simulation at (D-1 & D-2) below. For the Control geometry tab, we are using a predefined region in the same manner as we did above for the 3 Axis Horizontal Roughing. This time however, we have selected the Slot Bottom region. Also from the Control Geometry tab we have selected the Start Points sub-tab and then picked the Select Start Points button to add the point geometry we modeled to this operation (see CAD Geometry above). This will force the cutting to start at the top of our predefined thru hole location. 

This is considered a roughing operation because on the Cut Parameters tab we have Stock set to 0.2. This will leave 0.2 of material around the side walls of the bottom level of the keyway. Other cut parameters include an Offset cut pattern, a Mixed cut direction, and a stepover of 25%.

(D-1) Here we see the 2½ Axis Pocketing operation toolpath. It rough cuts the bottom level of the keyway slot.

(D-2) Here we see the cut material simulation showing the in-process stock remaining after the 2½ Axis Pocketing operation is completed.

Finishing Operations

The remaining two operations in the Machining Job are considered finishing operations. They are a 2½ Axis Profiling and a 2½ Axis Engraving operation. The 2½ Axis Profiling MOp is used to finish the side walls of the bottom level of the keyway slot. The Control Geometry tab of this operation is assigned the same pre-defined region (Slot Bottom) as the previous 2½ Axis Pocketing operation. 

For Cut Parameters the Tolerance is set to 0.01 and Stock is set to zero and Cut Direction is set to Mixed. For Cutting Side, the Determine using 3D Model is checked. The option Use Mid-Point of Longest Side is also checked which will move the start point to the our pre-drilled thru hole location. For the Cut Levels tab, the Location of Cut Geometry is set to At Bottom and the Total Cut Depth, Rough Depth, Finish Depth, Rough Depth/Cut and Finish Depth/Cut are all set to zero. This will produce one cutting pass at the bottom of the keyway slot. You can see the toolpath and the cut material simulation at (E-1 & E-2) below.

(E-1) Here we see the 2½ Axis Profiling operation toolpath. It finish cuts the side walls on the bottom level of the keyway slot.

(E-2) Here we see the cut material simulation showing the in-process stock remaining after the 2½ Axis Profiling operation is completed.

The final finishing operation is the 2½ Axis Engraving. This operation completes the keyway slot by machining the 5 degree ramp and finishing the side walls of the upper counterbore at the same time. From the Control Geometry tab we have selected the remaining two predefined regions. Also note the order of the regions in the Control Geometry tab. The Slot Ramp Outer region is listed first. This region will control the location of the tool at the cut start point. The Slot Ramp Inner region is listed second. 

 

 

When the cutter reaches the end point of Ramp Slot Outer it will immediately continue cutting from the start point of Slot Ramp Inner and then proceed to its end point to complete the operation. You can see the toolpath and the cut material simulation at (F-1 & F-2) below.

In 2½ Axis Engraving the center tip of the cutting tool (6.33 Diameter Glass/Carbon 46264 Flat End Mill) will follow the assigned control geometry exactly. In this case the predefined regions that we have created are driving the cutter to produce the finish cut of the 5 degree ramp at the base of the counterbore (on each side)! 

(F-1)Here we see the 2½ Axis Engraving operation toolpath. It finish cuts the 5 degree ramp and side walls on the top level of the keyway slot.

(F-2) Here we see the cut material simulation showing the in-process stock remaining after the 2½ Axis Engraving operation is completed.

 

The Cut Parameters tab simply states that the Tolerance is 0.01, the Cut Direction is Natural (meaning it is following the direction of the predefined regions), Location of Cut Geometry is At Bottom, all Cut Depth Control values are set to zero (one pass). For entry and exit both are set to None. From the Advanced Cut Parameters tab, Arc Fitting tolerance is set to 0.02.

Polar Instancing

The last item in the Machining Job tree is called Polar Instance 3@360 Degrees. As the name suggests this folder contains a copy of the six operations described above and defines the polar instance for the remaining three keyway slots. David can generate the gcode needed for all 4 keyway slots by simply posting out the Polar Instance.

 

3 Polar Instances of all 6 operations spanning 360 Degrees

 

Optional Methods

As we all know there are different approaches and methods to complete any CAM project. You may have already thought of a few while reading this article. We have to and would like to share a few of them with you here.

  1. Use native CAD system Curves instead of Curve Regions:
    In the Add Machining Regions section above we used MecSoft CAM regions derived from the native CAD system’s curve geometry. There is a reason for this. (a) We wanted to show you how to use Regions. (b) At times it can be easier to define, edit and select Regions rather than rely on the native CAD system to do this.

    However, we could have skipped the Add Machining Regions section, and simply selected the native curves as Control Geometry. However, we would have needed to make sure the curve start points are correct. In RhinoCAM you can use the Mark Curve Start command (CrvStart) to do this. In VisualCAD/CAM you would use the Reverse Curve Direction command located on the Curve Modeling tab if the curve start point is incorrect. 
  2. Use 3 Axis Parallel Finishing instead of 2 Axis Engraving: We could have used the 3 Axis Parallel Finishing method but would have had to settle for less control of the cutter. Again, in 2½ Axis Engraving, the tip of the cutter follows the control geometry (i.e., the curve regions) exactly. There is no greater control than this.
  3. Reverse the direction of Slot Ramp Inner:
    If you look closely at the illustration below, you will notice that the start point of the Slot Ramp Inner predefined region is located at the end point of Slot Ramp Outer causing the cutter to ramp downward, cutting with the flat bottom of the cutter during the 2½ Axis Engraving operation. This is not ideal. If we reverse the direction of this curve region, the cutter will ramp upward, allowing the tool to cut along it’s flute length.

 

Illustration showing the cut direction of the 2½ Axis Engraving operation.

 

Cool Project David!

Thank you for allowing us to showcase your work at Jim Thompson Marine Carpentry!

 

More about Jim Thompson Marine Carpentry

From new decks to custom cabinetry, Newport Shipyard’s carpentry shop, managed by J. Thompson Marine Carpentry, produces the highest quality woodwork on every new build and refit. All carpenters and craftsmen are versed in the widest range of materials, methods and technologies, be it wood, Corian, or composite from new to classic yacht restoration. The right fit and finish is a constant at Newport Shipyard!

 

Newport Shipyard’s carpentry shop, managed by J. Thompson Marine Carpentry

August 26, 2021
26 Aug 2021

RhinoCAM Teacher/Student Project with Rhino Education Specialist Pete Sorenson

Pete Sorenson has spent 42 years teaching technology classes to High School students at Lake Washington High School, Kirkland Washington as well as the greater Kirkland Washington area and the Rainier School District in Rainier OR. Pete’s curriculum has included AutoCAD & Drafting, Automotive Shop, WoodShop and Metal Shop. Currently, Pete is one of three Education Specialists with McNeel & Associates who actively run technology workshops educating teachers on the use of CAD/CAM technology including the Rhinoceros CAD (Rhino) drawing and modeling program. 

Pete’s hand-on workshops teach educators how to draw in 2D and how to model in 3D using Rhino, how to design for manufacturing, how to setup their CNC machines, how to hold and fixture parts and most of all, how to get projects completed using CNC mills, routers, 3D printers and more.

 

The RhinoCAM Difference

Pete also performs custom CNC manufacturing for an exclusive set of clients including fixtures and tooling for manufacturing custom cutting tools, hydroplane water racing craft components and automotive street racing applications. Pete also performs custom machining on some of the oldest street clocks in America, many currently in museums! In his home workshop Pete uses RhinoCAM to generate G-Code for his ProLite CNC mill. Also included are 3 manual lathes, 3 milling machines, band saws, drill presses, and a metal-working shaper! 

We recently sat down with Pete to discuss his amazing career and to ask him why RhinoCAM is his goto program for generating G-Code and for teaching other educators to use CNC machining technology. Here is just some of what Pete had to say about his RhinoCAM

What sets RhinoCAM apart from other CAM systems?

“Well, there is good support #1, good price #2, and once you get the vernacular of what the different menus are asking you to do its relatively easy #3! Also, the fact that you can edit your Rhino drawing and then go directly to RhinoCAM to update your toolpaths makes it very flexible especially with multiple monitors.”

Pete Sorenson, Education Specialist
McNeel & Associates, Kirkland, Washington

 

The RhinoCAM Student Project

In this project teachers and students learn the basics of RhinoCAM by programming 2½ Axis Pocketing and 2½ Axis Profiling operations to machine the letter tile block shown here on the right. The exercise illustrates the use of simple 2D geometry to define setup and stock parameters as well as the ability to cut pockets for roughing and Profiles for finishing. There are similar tiles for each letter in the alphabet so teachers and students select combinations of tiles to complete a project. 

 

The CAD Geometry

The CAD geometry for this project is simple planer 2D curves drawn on the default Rhino XY construction plane (from the Top View) as shown in the illustrations below. All of the curves are located on this default XY Plane. The outer rectangle is 3” x 3” square and represents the outer perimeter of the tile. The bottom left corner of this rectangle is located at the WCS (World Coordinate System) 0,0,0 origin. We will refer to this as “XYZ” zero. That is because this default construction plane is located at a Z depth of zero and the bottom left corner of the geometry is located at XY zero.

 

The illustration above shows the 2D curve geometry that will be used for this project. All dimensions are for reference only and are not used in the CAM project. The curves are located on Rhino’s default XY plane. You can show this plane by selecting the Top View in Rhino.

Here we see the default Perspective view in Rhino. It shows that all geometry is located on the default XY construction plane with the bottom left corner located at the WCS (World Coordinate System) 0,0,0 origin.

The Stock & Setup

The stock definition in RhinoCAM for this project is a Box Stock with Length (L) equal to 3.00”, Width (W) equal to 3.00” and Height (H) equal to 0.75”. Notice that the top right corner of the stock in the dialog below is selected. This means that the dimensions entered into the dialog are measured from this corner of the box stock. Also, under Corner Coordinates you see that Xc, Yc and Zc each equal zero. That corresponds with the lower left corner of our control geometry which by default is the WCS (World Coordinate System) origin. The setup or workpiece origin is located at this 0,0,0 position.

For the project’s limited piece runs, Pete uses blue tape and super glue to hold the blocks to the fixture on the milling table. Pete also uses ORACAL Oramask 813 Stencil Film to mask the top of the stock prior to machining. 

Pete recommends using a 2-flute down cut ⅛” diameter flat end Mill (from 2Linc.com) at a cut feed rate of 10 in/min for each of the 2½ Axis Pockets and Profiles. This tool in combination with the ORACAL Oramask 813 Stencil Film provides very clear and sharp edges that shear the Oramask eliminating “paint bleed” under the masking. See more finished letter tile block images below!

 

The Box Stock dialog shows the Corner Coordinates to be located at 0,0,0 and the stock dimensions to be 3”x3”x0.75”.

The Box Stock values in the dialog on the left will preview the stock size and location on the part. Notice that the bottom/left corner of the stock is located at 0,0,0 (the World Coordinate System) origin.

 

Sequence of Operations

The Machining Job and Setup 1 shown here on the right includes one 2½ Axis Pocketing operation followed by three 2½ Axis Profiling operations. All four operations use the same tool which is a down spiral ⅛” diameter Carbide 2 Flute Flat End Mill.

Setup 1 shown in the Machining Job is located at the WCS origin (0,0,0). You can locate this position in the illustrations above. When you post Setup 1, each machining operation is then posted in the order that they appear under Setup 1. See Posting G-Code below for more information on posting options.

 

2 1/2 Axis Pocketing 1 (FM: 1/8″ 2F CARB)

The first machining operation that appears under Setup 1 is 2 1/2 Axis Pocketing 1 (FM: 1/8″ 2F CARB). It performs a pocketing operation to clear stock material out between the two closed curve regions shown here on the right. The resulting toolpath and many of its Cut Parameters are shown in the illustrations below.

For Cut Parameters the Global Tolerance for the operation is 0.001”, a Stock value of 0.025” and cutter compensation is disabled. This means that there will be a thickness of 0.025” left between the cutter diameter and the curve regions. The tool path employs an Offset cut pattern, a Climb cut direction, an Inside start point, and a Stepover of 25% of the tool diameter.

 

In this illustration we see the cut material simulation and tool paths for the first cut level of the 2½ Axis Pocketing operation. Many of the Cut Parameters are labeled as well as the entry and exit motions.

 

This Pocketing toolpath contains three cut levels. The Total Cut Depth is set to 0.093” with the Depth per Cut set to 0.033”. Each cut level has a 10 degree ramp entry. The elevation view of the cut material simulation is shown in the image below. The control geometry (2D closed curves) are located at Z zero as indicated by the WCS triad on the left. The area below Z zero is the stock geometry.

In this elevation view we see the results of the cut material simulation of the 2½ Axis Pocketing toolpath operation. The 10 degree ram entries are clearly shown as well as each cut level.

 

2 1/2 Axis Profiling 1 (FM: 1/8″ 2F CARB)

The second operation in the Machining Job tree is 2 1/2 Axis Profiling 1 (FM: 1/8″ 2F CARB). This is a Profiling operation used as a finishing cut around the inner side of the closed curve perimeter of the pocket. The control geometry selected for this operation is shown in the illustration on the right.

For Cut Parameters the Global Tolerance for the operation is 0.001”, a Stock value of 0 (zero) and cutter compensation is disabled. This means that the diameter of the cutter will touch the perimeter curve and follow it along the inner side of the previous pocketing operation. The Cut Direction is set to Climb and the Cutting Side is set to Inside. The Total Cut Width is set to zero. This means that the cutter will not offset in the XY direction. The cutter will ramp at a 10 degree angle into the stock material at the cut start point and will travel around the curve and then perform a vertical retract when it passes the cut start point by 0.2”. The cut level parameters are similar to the 2½ Axis Pocketing elevation view shown above. 

In this illustration we see the cut material simulation and tool paths for the first cut level of the first 2½ Axis Profiling operation. Many of the Cut Parameters are labeled as well as the entry motion.

 

2 1/2 Axis Profiling 2 (FM: 1/8″ 2F CARB)

The third operation in the Machining Job tree is 2 1/2 Axis Profiling 2 (FM: 1/8″ 2F CARB). This is the second Profiling operation used as a finishing cut around the outer side of the closed curve perimeter of the letter “H”. The control geometry selected for this operation is shown in the illustration on the right.

The Cut Parameters are nearly identical to the previous Profiling operation. One difference is that the Cutting Side is set to Outside. Another difference is that on the Cornering Parameters tab, the External Corner Type is set to Sharp. This means the cutter will not roll around the 90-degree corners but will travel past the corner and then make a 90-degree turn. These sharp corners are labeled in the illustration below. This method results in a precise sharp corner where needed. The Cut Direction, Cutting Side, Ramp Entry, Vertical Retract and Cut Levels are all identical to the previous Profiling operation. The cut material simulation for the first of three cut levels in this operation is shown below.

In this illustration we see the cut material simulation and tool paths for the first of three cut levels in the second 2½ Axis Profiling operation. The 10-degree Ramp Entry can be clearly seen as well as the External Sharp Corner option.

 

2 1/2 Axis Profiling 3 (FM: 1/8″ 2F CARB)

The final operation in the Machining Job tree is 2 1/2 Axis Profiling 3 (FM: 1/8″ 2F CARB). This is the third Profiling operation used as a finishing cut around the outer side of the closed curve boundary surrounding the letter “H”. The control geometry selected for this operation is shown in the illustration on the right.

The Cut Parameters, Cornering Parameters, Cut Levels and Entry/Exit parameters are identical to the previous Profiling operation shown above. The Cut Direction, Cutting Side, Ramp Entry, Vertical Retract and Cut Levels are shown in the cut material simulation illustration below. 

 

In this illustration we see the cut material simulation and tool paths for the first of three cut levels in the third 2½ Axis Profiling operation. The 10-degree Ramp Entry and the External Sharp Corners are clearly visible.

Other Operation Parameters

The dialogs below shows the Feeds & Speeds parameters as well as the Clearance Plane parameters. These are identical for all of the operations in this setup.

 

Here we see the Feeds & Speeds parameters and the Clearance Plane parameters. They are identical for all 4 operations under Setup 1 in this Machining Job.
Cut Material Simulation

The animation below illustrates the complete cut material simulation for all 4 operations under Setup 1 in the Machining Job. It begins with the 2D drawing, and then shows the stock model overlay and then proceeds to simulate each operation starting with 2½ Axis Pocketing followed by each of the three 2½ Axis Profiling operations. 

Here is the cut material simulation for all 4 toolpath operations under Setup 1. It begins with the 2D drawing, and then shows the stock model overlay and then proceeds to simulate each operation starting with 2½ Axis Pocketing followed by each of the three 2½ Axis Profiling operations.

 

Posting G-Code to the ProLite CNC Mill

With our toolpath operations complete and we are satisfied with our Cut Material Simulation we can start posting G-Code to the ProLite CNC Mill. RhinoCAM provides flexibility in how you want to post your G-Code. You can post the entire setup by selecting Setup 1, right click and pick Post from the popup menu. Since all 4 operations use the same cutting tool, this method will work fine. You can refer to the illustrations below. 

(Left) Right-click on Setup 1 from the Machining Job tree and select Post to create one G-Code file that contains all 4 operations. (Right) Here we see the G-Code file displayed in Notepad. The first 2½ Axis Pocketing operation is highlighted.

 

Alternatively, you can post one or more operations at a time into one or more G-Code files. Just press and hold the <Ctrl> key while you select multiple operations and then right-click and select Post from the popup menu. Only the select operations will be posted to the G-Code file. Again, you can refer to the illustrations below.

(Left) To post multiple operations at one time, while pressing the <Ctrl> key select the operations from the Machining Job tree and then right-click and select Post. (Right) Here we see the G-Code file displayed in Notepad. The first 2½ Axis Profiling operation is highlighted.

 

Machining Pics

Here are some cool images of the letter tile blocks after masking and machining and then before and after painting. 

 

Here is the part still on the CNC machine prior to painting with the ORACAL Oramask 813 Stencil Film still attached.

Here are the letter tiles after painting after removing the ORACAL Oramask 813 Stencil Film.

 

Cool Teacher/Student project Pete!

Thank you for allowing us to showcase your work!


More about Pete Sorenson

Pete Sorenson is a retired High School High School technology instructor from Kirkland, Washington. Currently Pete is one of three Education Specialists with Robert McNeel & Associates in Seattle, WA performing Rhinoceros CAD and Rhino plugin workshops for educators at all levels. Pete has been a RhinoCAM user since the product’s release in 2002 and runs his own shop providing CNC services for an exclusive list of clients including Eastside Tooling.com. Pete’s current cool project is restoring the inner working components for the 36” diameter historic Carol’s Clock located in the Museum of History & Industry on the shores of Lake Union. Pete recommends all educators and students to visit the Rhino Education Resources page here. You can reach out to Pete Sorenson at pete@mcneel.com.

 

The historic Carol’s Clock located at the Museum of History & Industry (MOHI) on the beautiful shores of Lake Washington

 

More about Robert McNeel & Associates & Rhino

Robert McNeel & Associates, founded in 1980, is a privately-held, employee-owned company with development, sales support, training offices, and affiliates in Seattle, Boston, Miami, Medellin, Barcelona, Rome, Tokyo, Taipei, Seoul, Kuala Lumpur, Beijing, Shenzhen, and Shanghai. We also have more than 700 dealers, distributors, OEMs, and training centers around the world. 

Rhino geometry is based on the NURBS mathematical model, which focuses on producing mathematically precise representation of curves and freeform surfaces in computer graphics (as opposed to polygon mesh-based applications). Rhinoceros is developed for the Microsoft Windows operating system and macOS.

Robert McNeel & Associates
Headquarters, North America, and Pacific
3670 Woodland Park Ave N
Seattle, WA 98103 USA
Main: +1 (206) 545-7000
Sales: +1 (206) 545-7000
Support: +1 (206) 545-6877


Follow Robert McNeel & Associates Online:

August 19, 2021
19 Aug 2021

Basic Masking & Fixture Tips from Pete Sorenson

Pete Sorenson has spent 42 years teaching technology classes to High School students at Lake Washington High School, Kirkland Washington as well as the greater Kirkland Washington area and the Rainier School District in Rainier OR. Currently, Pete is one of three Education Specialists with McNeel & Associates who actively run technology workshops educating teachers on the use of CAD/CAM technology including the Rhinoceros CAD (Rhino) drawing and modeling program. 

 

For the one-off and limited production environment of home and education workshops Pete suggests using blue masking tape and super glue to hold wood blocks to the fixture board on the milling table. If the block will be painted after machining, Pete also uses ORACAL Oramask 813 Stencil Film to mask the top of the stock prior to machining. Below is an example of this procedure.

 

In the above example, Pete covers the top of the stock with ORACAL Oramask 813 Stencil Film and the bottom is attached to the milling table with blue masking tape and super-glue. This combination along with the 2-flute down cut ⅛” diameter flat end Mill (from 2Linc.com) placing consistent down cut pressure on the stock during machining.

 

In the above example, Pete covers the top of the stock with ORACAL Oramask 813 Stencil Film and the bottom is attached to the milling table with blue masking tape and super-glue. This combination along with the 2-flute down cut ⅛” diameter flat end Mill (from 2Linc.com) placing consistent down cut pressure on the stock during machining.

 

Here are the letter tiles after painting after removing the ORACAL Oramask 813 Stencil Film.

 

More about Pete Sorenson

Pete Sorenson is a retired High School technology instructor from Kirkland, Washington. Currently, Pete is one of three Education Specialists with Robert McNeel & Associates in Seattle, WA performing Rhinoceros CAD and Rhino plugin workshops for educators at all levels. Pete has been a RhinoCAM user since the product’s release in 2002 and runs his own shop providing CNC services for an exclusive list of clients including Eastside Tooling.com

August 11, 2021
11 Aug 2021

MecSoft Partners with Mecanumeric

Dana Point, CA, August 11, 2021: MecSoft Corporation, the developer of industry leading CAM software, has announced today a partnership with Mecanumeric, a leader in CNC milling machines. As part of this partnership, Mecanumeric will be bundling MecSoft’s VisualCAD/CAM and RhinoCAM products with their milling and turning machines.

“We are thrilled to announce that Mecanumeric will be bundling MecSoft’s CAM products with their milling and turning machines. We look forward to working with the team at Mecanumeric to bring to market the best of class CAD/CAM and CNC machining solutions.” says Joe Anand, President & CEO of MecSoft Corporation.

Arthur Pais, MECANUMERIC President and CEO explains: “With this cooperation with MecSoft, we will have a reliable, evolutive and versatile CAD/CAM solution which allows us to offer a full manufacturing solution including our large range of machine for a wide panel of worldwide customers, from basic needs (schools) to very high level requests (aircraft industry)”.

 

 

About Mecanumeric

Mecanumeric offers a wide range of CNC solutions highly recognized in the industrial, dental and education fields. With a vast portfolio of milling, waterjet cutting machines, laser cutting and engraving, turning, vacuum forming, knife and ultrasonic cutting solutions, Mecanumeric can address various markets: SIGN and POPAI, Education and Fablabs, Building, Furniture and Decoration, Aircraft and space Industry, parts prototyping, plastics… 100% of engineering, manufacturing and service (installation, training, parts and consumables sales, aftersales service…) take place internally, from its facilities in France to all across Europe and beyond.

For more information, visit www.mecanumeric.com or call (0033) 563 383 440.

 

 

About MecSoft Corporation

Headquartered in Dana Point, California, MecSoft Corporation is a worldwide leader in providing Computer Aided Manufacturing (CAM) software solutions for the small to mid-market segments. These solutions include the products VisualCAD/CAM®, RhinoCAM™ and VisualCAM for SOLIDWORKS®. 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.

July 23, 2021
23 Jul 2021

MecSoft Announces Service Packs For All Its 2021 Products

Dana Point, CA, July 21, 2021:  MecSoft Corporation, the developer of computer aided manufacturing (CAM) software solutions, has announced service pack releases for all its 2021 versions of CAM products.

These Service Packs were released in order to add some minor enhancements and to fix some bugs. All products have undergone rigorous testing and have been certified to be production ready.

For a complete list of changes please visit the Product download pages.
Free demo software of our products can be downloaded at http://mecsoft.com/downloaddemos

For more information, please visit mecsoft.com or call (949) 654-8163.

About MecSoft Corporation

Headquartered in Dana Point, California, MecSoft Corporation is a worldwide leader in providing Computer Aided Manufacturing (CAM) software solutions for the small to mid-market segments. These solutions include the products VisualCAD/CAM®, RhinoCAM™ and VisualCAM for SOLIDWORKS®. 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.

June 8, 2021
08 Jun 2021

CAMJam 2021 is Here!

MecSoft Corporation is proud to announce the release of CAMJam 2021, the Video & Document Training Companion set for our popular VisualCAD/CAM®, RhinoCAM® and VisualCAM® for SOLIDWORKS CAM modules. This year we packed CAMJam full of new videos for each CAM module including the 2021 AMS bonus modules Profile-NEST and G-Code Editor as well as continued easy access to all available resources! 

What’s inside CAMJam 2021

CAMJam 2021 now includes over 150 instructional videos covering the complete suite of the MecSoft CAM module functionality including MILL, TURN, NEST, ART, Profile-NEST, G-Code Editor and MESH! The set includes the CAMJam 2021 PDF Guide document that indexes and links directly to the content within each video so you know exactly what (and where) to watch to get your questions answered.

Here is a list of what you will find in CAMJam 2021:

  • Learn about all of the new functionality in MecSoft’s 2021 version CAM Plug-ins.
  • Must Watch Bonus Videos including best practices in 2½ and 3 axis machining, CAM Coordinate Systems Explored, Mold and Parting Line Machining, Machining Multi-Sided Parts and more.
  • VisualCAD Mash-up with links to every video subject that discusses MecSoft’s free drawing program.
  • All of the MILL Module features including Fundamentals, Feature Detection Machining, 2½, 3, 4 and 5 axis machining.
  • More videos on machining scan meshes, machining nested sheets and more!
  • Links to the popular must-read MecSoft Tech Blog learning articles as well as the latest in-depth case studies of users like you, who are achieving success with their MecSoft CAM software.
  • Bonus Guides and Tutorials. That’s right, CAMJam 2021 includes access to exclusive materials including The CAM Question & Answer Guide and the Cutting Tools Workbook, all updated for MecSoft’s 2021 lineup of CAM module plug-ins! 
  • The CAMJam 2021 User Guide for the organization and easy retrieval from the video and document library.

 

Exclusive Bonus Guides

CAMJam 2021 includes exclusive guides and tutorials only available to MecSoft annual maintenance subscribers (AMS). These training guides are not available anywhere else! Also included are videos and guides on each of the 2021 AMS Bonus modules including Profile-NEST and the popular G-Code Editor!

 

The MecSoft CAM 2021 Question & Answer Guide

The MecSoft CAM Question & Answer Guide contains concise information so that you learn quickly. Each question is answered with the menu selections required to complete the task and illustrations to help you understand the results. 

Here are just a few examples of what’s included:

  • Enable Cutter Compensation
  • Enable Inverse Time Feed Rate
  • Define Toolpath Properties
  • Accurately Estimate Machining Time
  • Edit Toolpaths Associatively
  • Add a Tool Change Point
  • Add more Materials
  • Add Tool Comments
  • Find Tool Related Preferences
  • Load a Tool Library Automatically

 

The 2021 Cutting Tools Workbook

CAMJam now includes the newly updated 2021 Cutting Tools Workbook. This guide walks you through the process of creating tools and using the predefined tool libraries installed with the software as well as creating your own custom tool libraries. Also included is in-depth information on the Tools tab and the Create/Select Tools dialog including the Feeds & Speeds Calculator!

This guide also includes worksheets on every tool type supported by the 2021 MILL and TURN modules! You can print these worksheets and use them to document your existing and new tool inventory for creating tools and setting up your tool library in the MecSoft CAM plugin of your choice! 
 

The 2021 F1 CO2 Racer Body Tutorial

Back by popular demand, CAMJam includes the F1 CO2 Racer Body Tutorial newly updated for each MecSoft 2021 desktop CAM plugin. This tutorial walks you step-by-step through the process of setting up and machining the Racer Body in a two-sided machining process also referred to as flip machining using both 2½ Axis and 3 Axis toolpath strategies. This tutorial includes comprehensive illustrations to help guide beginners through the process of creating toolpaths.

The tutorial will illustrate how to machine the F1 CO2 Race Car body from a balsa wood stock blank. The stock can be machined from the Pitsco Custom Cruiser Blank SKU: W17823 or the blank included with the Pitsco Custom Cruiser Vehicle Design Kit SKU: W54600
 

To get your Annual Maintenance Subscription

To learn more about being an AMS subscriber and CAMJam just give us a call, chat or contact MecSoft sales and/or support. We will be happy to give all of the details.
 

More articles about CAMJam

 

More about MecSoft CAM Products

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:

June 2, 2021
02 Jun 2021

How to Migrate Your CAM Data from AlibreCAM to VisualCAD/CAM

Being an AlibreCAM user you likely know now that AlibreCAM’s last supported version in AlibreCAM 2020 and that all AlibreCAM users are being migrated to VisualCAD/CAM. This is a free migration to all AlibreCAM users. As an AlibreCAM user, you will need to migrate all of your AlibreCAM data files to VisualCAD/CAM to continue to access your embedded CAM knowledge. The good news is that AlibreCAM already includes a migration tool that will export your Alibre Design, including all CAM data to VisualCAD/CAM! 

The procedure to convert your AlibreCAM data files is provided below.

Please note that you MUST migrate all of your existing Alibre Design/AlibreCAM files over to VisualCAD/CAM in order to continue to access your existing CAM knowledge!

You can follow the steps outlined below to use the Export to VCP utility located in AlibreCAM. The complete Alibre Design part geometry as well as all AlibreCAM toolpaths will be migrated for you. If you have any difficulty migrating your CAM data, please contact us at support@mecsoft.com for assistance.

Steps to Convert AlibreCAM data to VisualCAD/CAM Data

1. Open Alibre Design and load the part file with CAM data that you want to export.

2. Load the AlibreCAM plugin and load the MILL module.

 

 

3. Your AlibreCAM data looks like this:

 

 

4. From the AlibreCAM Machining Browser locate the Utilities menu and select the Export to VCP command.

 

 

5. Enter a name for the new VCP (VisualCAD/CAM) part file and pick OK.

6. Run VisualCAD/CAM and load the MILL module.

7. In VisualCAD/CAM, from the File Open dialog, navigate to the VCP file that you just exported from AlibreCAM and pick OK. The file is opened in VisualCAD/CAM and includes all geometry, all machining operations and all tools.

 

 

For More Information

If you have any questions about your AlibreCAM data please do not hesitate to contact MecSoft Customer Support online at https://mecsoft.com/request-support/ or via email at support@mecsoft.com

More about MecSoft CAM Products

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

May 17, 2021
17 May 2021

Get the 2021 Cutting Tools Workbook!

MecSoft Corporation is excited to announce the release of The 2021 Cutting Tools Workbook, a 120-page guide to working with cutting tools in its line-up of CAM plugins including VisualCAD/CAM, RhinoCAM and VisualCAM for SOLIDWORKS MILL, TURN, Profile-NEST and G-Code Editor modules. This is a bonus guide now free to all users. Many of you have asked for more comprehensive information on working with Cutting Tools in our CAM module plugins. This updated workbook delivers the following in-depth information.

 

Creating Tools

This guide walks you through the process of creating tools and using the predefined tool libraries installed with the software as well as creating your own custom tool libraries. Also included is in-depth information on the Tools tab and the Create/Select Tools dialog including the Feeds & Speeds Calculator!

 

The Create/Select Tools Dialog

 

Tool Related Answers

This updated workbook also includes answers to many of the questions that users ask most, including how to define a custom tool, print your tool list, define tool related preferences and tool related optimization such as machining time estimates and more.

 

Advanced Topics

This updated workbook also answers more advanced questions such as how to include tool comments, define a tool change point and enable cutter compensation in your posted g-code. How to customize the Feeds & Speeds Calculator with your own custom materials is also explained.

 

Worksheets

You may be asking yourself why is this guide called a workbook? That’s because it includes worksheets on every tool type supported by the MILL and TURN modules! You can print these worksheets and use them to document your existing and new tool inventory for creating tools and setting up your tool library in the MecSoft CAM plugin of your choice! A sample worksheet is shown below.

 

Sample MILL Tool worksheet from The Cutting Tools Workbook

 

Sample TURN Tool worksheet from The Cutting Tools Workbook

 

Data Sheets

In addition to the worksheets mentioned above, the Reference section also includes the parameter values of every INCH and METRIC tool that comes installed in the predefined tool libraries so that you know exactly which parameter to adjust to make them YOUR custom tool library!

 

What’s Inside

The Cutting Tools Workbook is packed full of information that will help you become more proficient with your MecSoft CAM software. Here is the complete list of topics included in this must-have companion guide.

What’s New
Videos & Guides
Print Media Archive

About This Guide
          About the MILL Module
          About the TURN Module
          Using this Guide

Getting Ready
          After Installing MILL
          Locate the Tools Tab
          The Create/Select Tools Dialog

Creating Tools
          Create a Tool
          Create a Tool Library
          The Feeds & Speeds Calculator
          Use The Preinstalled Tool Libraries
          Add your Existing Tools to a Library
          More about the Tools Tab
          More about the Create Tools dialog

Tool Related Answers
          Where can I find Tool Preferences?
          How can I Print a Tool List?
          How can I add a Custom Tool?
          Why are my Feed Rate values too High/Low?
          What about Tapping Feed Rates?
          Optimize Machining Time Estimates?

More Advanced Answers
          How to add Tool Comments?
          How to add a Tool Change Point?
          How to add more Materials?
          How to enable Cutter Compensation?

Reference
          Mill Tool Worksheets
          Drill Tool Worksheets
          Turn Tool Worksheets
          Feeds & Speeds Data
          Default English Tools Library
          Default Metric Tools Library

 

How to Download this Guide

This tutorial is available as a FREE download to ALL MecSoft CAM users. To download this 110-page guide, select from one of the links below for your MecSoft product:

 

RhinoCAM 2021 VisualCAM 2021 VisualCAM 2021 for SolidWorks

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:

May 12, 2021
12 May 2021

Indexed Machining with MecSoft CAM

MecSoft is proud to introduce the latest addition to its 3 Axis advanced machining suite, Indexed 3+2 Machining. This advanced Multi Axis method can be added, as a separately priced module, onto any Standard or Expert configuration. That’s right, you don’t need to have the Professional or Premium configurations to get the benefits of Indexed 3+2 Machining!

 

What is Indexed Machining? 

Indexed machining allows you to lock in place (i.e., index) your 4th axis (referred to as 3+1) and/or your 5th axis (3+2), while performing 2 Axis and 3 Axis operations. Indexed machining also includes a host of other key benefits not available in 3 Axis or 3 Axis Advanced programming. For example, you can machine multi-sided parts in 3, 4 or 5 axis mode. Indexing the 4th or 5th axis means less manual setup reducing machining time and increasing machining accuracy.

 

Indexed 3+2 machining allows you to lock in place (i.e., index) your 4th axis (referred to as 3+1) and/or your 5th axis (3+2), while performing 2 Axis and 3 Axis operations.

 

Key Benefits

Indexed machining also includes a host of other key benefits not available in the Standard, or Expert configurations. These include:

 

Key Benefits of the Indexed 3+2 Addon Module

 

  • Machine Multi-Sided Parts & Improve Machining Accuracy:
    For example, you can machine multi-sided parts in 3, 4 or 5 axis mode. Indexing the 4th or 5th axis means less manual setup reducing machining time and increasing machining accuracy.
  • Reduce Tool Positioning Errors:
    Indexed 3+2 machining also reduces tool positioning errors by leveraging the accuracy of your CNC machine. Each indexed position eliminates a manual setup and tool positioning.
  • Save Programming Time:
    You can also save time by programming all sides of a part in one Machining Job. Toolpath simulation time is also reduced because all setups are included in one part file!

 

Key Features

A host of added features is really what makes Indexed machining shine. Take a closer look at these key features:

 

Machine Multi-Sided Parts with Ease!

You can easily machine any multi-sided part with ease. In the following example, a part that requires machining from three sides is programmed in one part file using multiple setups. Each setup can have its own independent Work Zero position. Without the Indexed Machining addon, each side would have to be programmed in separate part files, increasing complexity and chances for error. 

 

Machine Multi-Sided Parts with Ease!

 

Program and Simulate Toolpaths from Any Direction 

Once your multi-sided part is programmed, you will save additional time during cut material simulation because all setups are simulated in the same part file and in the actual setup sequence that will be performed on the cnc machine. Plus you’re not limited to simple parts. You can program even the most complex geometry using Indexed Machining techniques. 

 

Program and Simulate Toolpaths from Any Direction

 

Program Flip-Machining Jobs Using Indexed Machining

You can also program multi-sided flip machining utilizing that 4th axis. Referred to as indexed 3+1 machining, the 4th rotational axis automatically locks into place to machine each side, again without performing a manual setup. 

 

Program Flip-Machining Jobs Using 3+1 Programming

 

Perform XY and Polar Instance Programming!

Even if you are not utilizing your multi-axis capability, Indexed Machining includes many advanced 3 Axis features. For example, you can perform both XY and Polar instance programming. Again, program once and then let 3+2 do the rest!

 

Perform XY and Polar Instance Programming

 

If you need to machine identical components on multiple fixtures you can take advantage of the Fixture Offset Programming feature. Program once and then let Indexed Machining do the rest! 

Perform Fixture Offset Programming!

 

Perform Fixture Offset Programming

 

Perform 4th Axis Rotary Instance Programming!

If you need to machine identical components on multiple fixtures you can take advantage of the Fixture Offset Programming feature. Again, program once and let Indexed Machining do the rest!

 

Perform 4th Axis Rotary Instance Programming

 

Utilize Tombstone Tooling Blocks to Perform Multi-Part Indexing

You can also put that Tombstone Tooling Block to work programming multiple parts utilizing Indexed 5 Axis programming!

 

Utilize Tombstone Tooling Blocks to Perform Multi-Part 5 Axis Indexing

 

Perform Indexed Machining with Aggregate Heads!

You can put that Aggregate Head to work machining dowels, recessed pockets and mortising for cabinetry and other applications.

 

Perform Indexed 3+2 Machining with Aggregate Heads

 

Perform Advanced Machine Tool Simulations!

To wrap up this long list of features you can also perform advanced Machine Tool Simulation!

 

Perform Advanced Machine Tool Simulations

 

How to Get Indexed Machining

Indexed Machining can be added to either MecSoft CAM configurations: Standard or Expert for VisualCAD/CAM, RhinoCAM or VisualCAM for SOLIDWORKS. Contact our sales team (949) 654-8163 Option 1 today to get Indexed 3+2 Machining! 

 

More Information

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

April 26, 2021
26 Apr 2021

Introducing 3 Axis Adaptive Roughing!

MecSoft is proud to introduce the latest addition to its 3 Axis advanced machining suite, 3 Axis Adaptive Roughing. This advanced 3 Axis method can be added, as a separately priced module, onto any configuration starting with Standard (STD). That’s right, you don’t need to have the Expert, Professional or Premium configuration to get the benefits of 3 Axis Adaptive Roughing!

What is Adaptive Roughing? 

The Adaptive Roughing operation is a high speed bulk material removal toolpath method characterized by its tangential cut (i.e., constant cutter engagement) pattern. It reduces tool pressure and keeps chip load more consistent. It is especially valuable when cutting harder materials and generally results in much better tool life. Similar to Horizontal Roughing material is removed in layers or levels from the raw stock model. This is a constant contact toolpath method with just one entry and on exit at each cut level. Typical tools used for this kind of operation are Flat or Corner Radius mills. 

Key Benefits

3 Axis Adaptive Roughing offers the following key benefits not found on other 3 Axis roughing toolpath methods.

 

 

  • Consistent Cutting Conditions: With Adaptive Roughing there is only one entry and one exit for each cut level. You can also choose between Climb (down cut) or Conventional (up cut) meaning that the cutting condition of the tool remains consistent from start to finish for each cut level.
  • Increased Material Removal Rates: This method employs a High-Speed tangential cut pattern that facilitates the use of higher cut feed rates, making material removal fast and efficient. 
  • Reduced Cycle Times: The consistent cutting conditions and increased cut deed rates of the toolpath strategy results in much shorter cycle times even when more material needs to be removed.
  • Extended Tool Life: When combined, these benefits result in longer tool life so you will see a reduction in the purchasing in replacement tools. 
  • Reduced Stress on Machine Tool: In addition to longer tool life, this toolpath reduces rapid acceleration and deceleration in your machine tool, thereby increasing machining accuracy over the long run as reducing maintenance costs. 

 

Key Features

A wide range of features have been combined to make the 3 Axis Adaptive Roughing one of the smartest toolpath strategies in the MecSoft suite. The illustration below highlights these features on a sample part. Each feature is also illustrated below. 

 

 

Smart! Adapts to Part Features and Stock Conditions

Intelligence is designed into this Adaptive Roughing method. Your stock parameters and part features are analyzed and an adaptive roughing toolpath is generated to meet your specific needs. 

 

Smart! Adapts to Part Features and Stock Conditions

 

Spiral Engagements to Maximum Pocket Width

The maximum width of each pocket feature is calculated and a spiral path is employed. When this spiral path becomes constricted high speed tangential motions are added to maintain consistent cutting conditions. 

 

Spiral Engagements to Maximum Pocket Width

 

Corner Machining with Minimum Engagement Radius

When a corner feature is encountered a minimum engagement radius is calculated maintaining cut feed rate and minimizing cycle time.

 

Corner Machining with Minimum Engagement Radius

 

High Speed Cuts along Stock for Short Transfers

When short cut transfers are needed, the cutter will traverse along the stock perimeters at the cut feed rate minimizing cycle time even further. 

 

High Speed Cuts along Stock for Short Transfers

 

Adaptive Rest Machining between Levels

3 Axis Adaptive Roughing employs adaptive rest machining between levels. If stock remains on any portion of the part additional cut levels are added to remove it.

 

Adaptive Rest Machining between Levels

 

Step Minimization on Slopes and Contours

When Adaptive Roughing encounters a contour, Step Minimization is employed to further remove stock material. For example if the distance between cut levels is 50% of the cutting tool diameter, you can specify a lower cut level of say 25% that will automatically be employed along slopes and contours keeping the remaining in process stock to a minimum.

 

Step Minimization on Slopes and Contours

 

Cut Depths to Full Flute Length

In Adaptive Roughing the cutting tool will cut to it’s full flute length maximizing cutting levels and material removal.

 

Cut Depths to Full Flute Length

 

Depth/Level First Z Level Ordering

3 Axis Adaptive Roughing also employs Z Level ordering that allows you to control how cut levels are removed. Depth First will remove each pocket to its full depth before transferring to the next cut level. Level First will clear the entire level before moving to the next level.

Click here to enjoy the complete cut material simulation of this part.

 

Depth/Level First Z Level Ordering

 

How to Get 3 Axis Adaptive Roughing

3 Axis Adaptive Roughing can be added to any of the following MecSoft CAM configurations: Standard, Expert, Professional and Premium for VisualCAD/CAM, RhinoCAM or VisualCAM for SOLIDWORKS. Contact our sales team (949) 654-8163 Option 1 today to get 3 Axis Adaptive Roughing. 

 

3 Axis Adaptive Roughing Cut Material Simulation

 

More Information

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