Hole Machining in 2 & 3 Axis CAM Part 3: Automation

Welcome to our 4-Part series on Hole Machining in 2 & 3 Axis CAM using MecSoft’s CAM plug-ins. The complete 4-part Guide is available to all AMS subscribers as part of your CAMJam Self-Training package. See How to Download your CAMJam Training Materials for information about CAMJam and how to reap the benefits of your AMS subscription!

In the third installment of our series we explore Automation techniques that will help you get your hole geometry programmed faster. This section includes Feature Detection, Feature Machining, How to set a default AFM Knowledge Base, how to machine from that Knowledge Base and how to add hole features to a new Knowledge Base of your own.

The following 4 blog articles are included in this series:

1. Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
2. Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
3. Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
4. Hole Machining in 2 & 3 Axis CAM Part 4: Output Control

 

Hole Machining Automation

You can automate the task of generating a toolpath operation for a selected hole feature. During this process a toolpath operation is automatically selected from an Automatic Feature Machining (AFM) Knowledge Base, calculated and displayed. MecSoft CAM is installed with a predefined AFM Knowledge Base in both INCH and METRIC units. The topics below explain how the process works.

 

Hole Feature Detection & Machining

If your part file consists of a closed polysurface solid model, you can use hole feature detection and machining techniques to speed up the selection, classification and toolpath generation of your hole features. These commands and techniques are available from the Features tab of the Machining Objects Browser.

 

Detecting Hole Features

If the 3D model has hole features defined you can still use the selection techniques mentioned in Part 1: Hole Selection Techniques above. Alternatively you can use the feature detection tools on the Features tab of the Machining Objects Browser to detect your hole features.

Note that your part must be a polysurface solid model to use the Features tab options. You can set Diameter Range Filters from here also. Once hole features are identified, you can also manually execute a hole operation from the feature definition. First you need to detect your features.

Here are the basic steps to detect features:

1. Open the 3D polysurface solid model that contains hole features.

2. Select the Features tab from the Machining Objects Browser. If you do not see the Features tab, make sure the Machining Objects Browser is displayed.  There is a toggle located to the left of the Program tab. Select it until the Machining Objects Browser displays.

 

 

 

3. To set the diameter filter range, pick the  Set Filters for Feature Detection icon to display the dialog.

4. From the Global Filters tab make sure the box for Holes is checked.

 

 

5. From the Hole Feature Detection Filters tab check the box to Use diameter filter and enter the minimum and maximum diameters to select. There is also a box to Include Partial Holes if needed. Now pick OK to close the dialog.

 

 

6. The first two icons on the Features tab will detect features. You must use one of these two icons. The first icon will perform  Automatic Feature Detection (AFD). If you select it, ALL features in all orthographic orientation (not just holes) will be detected and added to your Features tree. They are also identified on your part geometry.

 

Detected Features List

Detected Features on Part

 

7. The second icon performs  Interactive Feature Detection (IFD) and allows you to detect features only from a selected flat area. This would be similar to using the On Flat Areas selection technique mentioned in Part 1: Hole Selection Techniques except that ALL features detect on the flat area will be added to your Features tree, not just holes. The features are also identified on your part geometry.

 

Detected Features List

Detected Features on Part

 

Note: If you do not see your features highlighted on the part go to CAM Preferences, select Features and make sure the box Turn on preselection highlighting is checked. CAM Preferences Dialog > Features

 

Hole Feature Types

The types of holes that are supported by AFM are any hole which has a cross-section that is made purely of straight line segments. In addition to this there cannot be any concave sections in the cross-section. The supported hole types are shown below.

 

 

Note all of these holes have straight line cross-sections with no concavities. In addition to this, the segments that make up a hole’s cross-section can be classified as 3 distinct types.

1. Vertical

2. Horizontal

3. Angled

The Angled segment is a segment that makes an angle between 0 and 90 degrees to the vertical. That is 0 < angle < 90. The reason for these three distinctions is that each type of segment will be machined in a similar manner. Thus Vertical segments may be drilled, horizontal segments may be spot-faced and angled segments may be machined with a tool of a similar angle.

 

Hole Feature Cross-Section Rules

The following rules are applied when a detected hole feature’s cross-section varies from those found in the Default AFM Knowledge Base.

 Rules when similar Hole Features are detected

ALWAYS perform a Cut Material Simulation after Automatic Feature Machining (AFM) to verify that the resulting toolpaths are what you are expect and desire. This should ALWAYS BE DONE before posting your toolpath!

 

Rules when a Similarity of Holes Diameters are encountered during AFM
Hole Types Supported
	Hole Pocketing & Profiling
	If the tool is smaller than diameter	Create the operation with the same tool.
	If the tool is larger than diameter	Create the operation with the same tool but mark the operation as dirty.
	Countersink
	If the tool is smaller than diameter & matches the chamfer angle	Create the program with the same tool.
	All other cases	Create the operation with the same tool but mark the operation as dirty.
	Drilling
	The tool matches the diameter exactly (within a user specified tolerance).	Create the operation with the same tool.
	The tool is larger or smaller than the hole diameter.	Create the operation with the same tool but mark it as dirty.
	Spot Drilling
	In all cases	Create the operation with the same tool but mark it as dirty.
	Spot Facing
	In all cases	Create the operation with the same tool but mark it as dirty.

 

Hole/Z Depth Rules when similar Hole Features are detected

ALWAYS perform a Cut Material Simulation after Automatic Feature Machining (AFM) to verify that the resulting toolpaths are what you are expect and desire. This should ALWAYS BE DONE before posting your toolpath!

 

Listing Hole Features

Once all of your hole features are detected they can be listed. Here is the procedure to obtain your hole feature list:

1. Open the 3D polysurface solid model file with hole features defined.

2. Detect your hole features. The procedure to do this is explained above. See Selecting Holes on a 3D solid model with hole features.

3. Once your hole features are listed in the Features tree, select the  List Features icon from the Features toolbar.

4. All of your features will displayed in the Machining Features Information table. The table will include information on Feature Type, Feature Name, and Feature Parameters. The Parameters column will contain the hole depth and minimum and maximum diameter dimensions. A Print button is provided if you with to print and save your list.

 

 

Machining Hole Features

You can only machine hole features AFTER the features are detected in your 3D solid model. See Detecting Hole Features above for the basic procedure to do this. Once your hole features are detected, you can execute the required hole operation directly from the feature definition.

Here are basic steps to do this:

1. First detect your hole features so that they are listed in the Features tree. The features tree is located in the Machining Objects Browser when the Features tab is selected.

 

 

2. Then right-click on a hole feature listed in the Features tree and select from the context menu of compatible toolpath operations. Only the operations that can be performed in the selected feature are listed in the menu.

 

 

3. Similarly, you can right-click on a hole feature that is detected and identified on your part model. By “identified” we mean that feature detection was performed and the hole feature displayed on your part model when you move the cursor over it.

 

 

4. If you do not see the feature highlighted, go to the Features section of the CAM Preferences dialog and make sure the box is checked to Turn on preselection highlighting. Also check the box to Turn on pre-selection information tooltips.

 

 

5. When the selected toolpath operation is executed, the hole feature information is automatically populated into the Hole Features tab of the toolpath operation dialog.

6. Complete the remaining tabs in the toolpath operation dialog and then select the Generate button to calculate and display the toolpath.

 

Set the Default AFM Knowledge Base

Before you can perform any Automatic Feature Machining (AFM) you should first check to make sure the correct AFM knowledge base is set. You can do this from the CAM Preferences dialog.

1. From the Machining Objects Browser select the CAM Preferences icon. It’s located on the top right end of the Machining Browser, next to the Help icon.

 

 

2. From the dialog select Features from the left side dialog menu.

3. Under the Automatic Feature Machining (AFM) Knowledge Base section locate the data field. It should show the folder location and file name of the AFM knowledge base.

 

 

Example: C:\ProgramData\MecSoft Corporation\RhinoCAM 20xx for Rhino x.0\FeatureBasedMachiningKBs\DefaultAFM_INCH.vkb

This example is pointing to the location of the default AFM knowledge base in inches for RhinoCAM. There is a similar file and location for VisualCAD/CAM, VisualCAM for SOLIDWORKS and AlibreCAM.

4. If the incorrect folder and/or file name is listed, select the “…” button to the right of the field to display the file browser.

5. Browse to the correct folder, select the DefaultAFM_INCH.vkb file and pick Open. If you work in metric units select the DefaultAFM_MM.vkb file and pick Open.

6. Now pick OK to close the CAM Preferences dialog.

 

Perform Hole Machining from a Knowledge Base

Here are the basic steps to automate hole machining using the default hole machining knowledge base:

1. First detect your hole features so that they are listed in the Features tree folder. The folder is located in the Machining Objects Browser when the Features tab is selected.

2. Then right-click on a hole feature listed in the Features tree and select Automatic Feature Machining (AFM) from the context menu. Alternately you can select the  Automatic Feature Machining (AFM) icon located on the Features tab toolbar.

3. You can perform the same procedure when you right-click on a detected hole feature directly from the 3D part model.

 

 

If you do not see the feature highlighted on the part, go to the Features section of the CAM Preferences dialog and make sure the box is checked to Turn on preselection highlighting. Also check the box to Turn on pre-selection information tooltips.

 

 

4. A Hole Feature MOpSet is added to the active setup in the Machining Job tree of the Machining Browser. If a hole feature match is found in the default hole machining knowledge base the machining operation created is generated automatically.

 

 

5. If the Hole Feature MOpSet created in the Machining Job is flagged, this means that no match could be found in the current default AFM knowledge base.

6. If this occurs, expand the Hole Feature MOpSet folder, right-click on the toolpath operation and pick Edit.

7. Select a tool and check the parameters in each tab of the operation dialog and pick Generate. The flagged should disappear. If it does not, check your parameters and try again.

 

Add Hole Features to the Default AFM Knowledge Base

Hole features are stored in the default AFM knowledge based on the cross-section dimensions of the hole. If an exact match (all diameters and depths of the hole) is found in the knowledge base it is used. You can add hole feature MOpSets to the default AFM knowledge base.

Here are the basic steps to edit the default AFM knowledge base:

1. First make sure the default AFM knowledge base is set. See: Set the Default AFM Knowledge Base for the procedure to check this.

2. Load the part file that contains the 3D solid model of the hole feature,

3. Detect the hole features in the part. You can use either the Automatic Feature Detection (AFD) command or the Interactive Feature Detection (IFD) command. Both are located on the Features toolbar. See: Detecting Hole Features above for this procedure.

4. From the Features tree select and right-click on the hole feature that you want to add to the knowledge base. You can also right-click on the detected hole feature directly from the 3D part model. If you do not see the feature highlighted on the part, go to the Features section of the CAM Preferences dialog and make sure the box is checked to Turn on preselection highlighting. Also check the box to Turn on pre-selection information tooltips.

5. From the context menu that displays select  Create Hole Feature for Machining KB. Alternatively, you can select the icon from the Features toolbar.

6. This will display the Select/Load/Create Operations for Matching Hole Feature dialog. This dialog allows you to assemble a MOpSet of toolpath operations to associate with the selected hole feature. For reference a cross-section of the selected hole feature is displayed along with its dimensions.

 

 

7. On the left side of the dialog you will see a list of toolpath operations that are compatible with the hole feature you have selected. Your hole feature is listed on the right. Consider how you want to machine the hole feature and then Drag & Drop the toolpath operations from the left to the right. Hint: Select and drag the folder of the toolpath operation past the vertical dividing line and drop it. It will locate itself under your hole feature folder.

8. Once you have all of the toolpath operations dropped into your hole feature folder, you can Drag them up or down in the list.

Note: In this dialog you are creating the MOpSet that will be executed when a matching hole feature is found. So make sure you arrange the toolpath operations in the order that you want then executed. For example if your hole feature is a counter-bore hole you may want the following operations listed in your hole feature folder:

 

 

9. When you are satisfied with your hole feature MOpSet (machining operation set), you can select one of the save buttons located at the bottom of the dialog.

Create Hole Feature MOpSet: Adds the MOpSet directly to your Machining Job.
Save as Knowledge Base: Saves the MOpSet to a new knowledge base file.
Save in AFM Knowledge Base: Adds the MOpSet to the current default AFM knowledge base defined in the CAM Preferences dialog.
Save in Knowledge Base: Select this button to save the Hole Feature and its Desired Operations into an (AFM) Knowledge Base file that is not set as the Default (AFM) defined in the Features section of the CAM Preferences dialog.

 

Add Hole Features to a New AFM Knowledge Base

You can also create a new AFM Knowledge Base.

1. See: Add Hole Features to the Default AFM Knowledge Base above and complete steps 1-8.

2. Pick Save as Knowledge Base.

3. From the File Save As dialog navigate to the folder where you want to locate your knowledge base file. Enter a name for the knowledge base and pick Save.

 

For more information:

1. Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
2. Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
3. Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
4. Hole Machining in 2 & 3 Axis CAM Part 4: Output Control

Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections

Welcome to our 4-Part series on Hole Machining in 2 & 3 Axis CAM using MecSoft’s CAM plug-ins. The complete 4-part Guide is available to all AMS subscribers as part of your CAMJam Self-Training package. See How to Download your CAMJam Training Materials for information about CAMJam and how to reap the benefits of your AMS subscription!

In part 1 of our series we explore all of the different techniques available for selecting geometry for hole machining. These techniques include selecting from 2D drawings, from a 3D surface and from a 3D solid model. You will also learn how to use the Diameter Range Filter coupled with selecting Holes on a Flat Area. You will learn about pre-defined regions, how to create them and use them as hole machining regions. You will also learn how to project the start point geometry to an irregular underlying 3D surface (for 3 Axis Hole Machining) from which each hole depth will be calculated from. And more…

The following 4 blog articles are included in this series:

1. Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
2. Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
3. Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
4. Hole Machining in 2 & 3 Axis CAM Part 4: Output Control

 

Hole Selection Techniques

Each hole machining operation, including Drill, Tap, Bore and Reverse Bore, provides multiple ways to select the control geometry that will define the Hole locations. For example, you can select just points, arcs, and/or circles. Like all toolpath strategies you can also select a region that you have previously defined (i.e., a predefined region) using the Regions tab of the Machining Objects Browser. You can also select holes automatically from a flat area or from hole features that you have previously detected in your model. Each of these methods are discussed below.

 

Selecting from a 2D Drawing

The hole geometry does not need to be completely defined in your part file. If you only have a 2D drawing you can draw points arcs or circles to locate your holes.

 

 

Selecting from a 3D Model

Similarly if you have a 3D model that does not have holes defined, you can still draw points arcs or circles to locate your hole operations. The geometry that you add can lie on the XY plane, located anywhere along the Z axis. Alternatively, the geometry can lie directly on the part model.

 

 

Selecting from a 3D Solid Model with Hole Features

If the 3D model has hole features defined you can still use the selection techniques mentioned above. Alternatively you can select the circular face edge defining the hole (or partial hole). You can also use the feature detection tools on the Features tab of the Machining Objects Browser to identify and locate your hole features.

 

 

 

Note: Your part must be a polysurface (i.e., solid) model to use the Features tab options. You can set Diameter Range Filters from here also. Once hole features are identified, you can execute the required hole operation from the feature definition.

 

Selecting Holes on Flat Areas

If your 3D model has a flat area that contains one or more holes (i.e., defined as complete and closed circles) you can use the Select Holes on Flat Area button located on the Hole Features tab of any of the hole operations (Drill, Tap, Bore or Reverse Bore). This option is very versatile and works if your flat area is a mesh, an open surface model or closed polysurface model.

 

 

Using the Diameter Range Filter

If you have many holes of different sizes, you can enable the Diameter Range Filter option located on the Hole Features tab of each hole operation dialog. Just check the box to enable the filter and then enter the minimum and maximum diameter to detect. When using the Select Holes on Flat Area button, only the hole edge geometry within these two range values are selected. Similar diameter filters are located on the Regions tab and the Features tab of the Machining Object Browser.

 

 

 

Using Predefined Hole Regions

You can predefine the hole geometry that you plan to use for any of the hole machining operation types by using the options on the Regions tab of the Machining Objects Browser. You can set Flat Area Region Selection Filters including Diameter Range Filters from here also.

Note: To use the Flat Area and Diameter Range Filters, you must have a flat area to select from. The flat area can be a 3D planar surface or planar mesh.

 

Here are the basic steps to create predefined regions for hole machining:

1. Open the part file with hole features defined. The part can be a 2D drawing, 3D surface or a polysurface solid model.

2. Select the Regions tab from the Machining Objects Browser. If you do not see the Regions tab, make sure the Machining Objects Browser is displayed.

 There is a toggle located to the left of the Program tab. Select it until the Machining Objects Browser displays.

 

 

 

3. To set the diameter range filter, select the  Flat Areas Selection Filter icon to display the dialog and check the box to User diameter filter and enter the minimum and maximum diameters to select.

 

 

4. Make sure the box to Ignore all inner regions is unchecked and then pick OK.

5. Now from the Regions tab pick the  Select Flat Areas icon.

6. Select a flat area from the part and then press Enter, right-click or pick OK.

 

 

7. A Machining Region Set is created and the detected hole regions are added to the set in the Machining Regions folder tree in the Machining Objects Browser.

 

 

 

8. Now select one of the Hole machining operations to display its operation dialog.

9. In the case of a Hole operation (i.e., Drill, Tap, Bore or Reverse Bore) from the Hole Features tab pick the Select Predefined button to display the selection dialog. In the case of 2 Axis Hole Pocketing or Hole Profiling, pick the Select Predefined button on the Control Geometry tab.

 

 

10. Select a Region or a Machining Region Set and then pick OK.

 

 

11. The regions are added to the Selected Holes list on the Hole Features tab and highlighted on the part.

 

 

Projecting Selections to Part Geometry

If you have an irregular surface that you want to drill into and still maintain a consistent hole depth in relative to the surface, you can enable the Project to 3D Model option. This is located in the Location of Drill Points group of the Cut Parameters tab of each hole operation dialog. This allows you to locate your drill points on an XY plane. The drill points will be projected to the surfaces and the Drill Depth will be calculated relative to the projected located on the surface. This is illustrated in the example below.

 

Project Drill Points to the 3D Model

 

Machining Partial Holes

You may encounter parts that require you to machine a partial hole. For example when a hole passes through multiple stepped levels of stock material. For selection purposes the partial hole must contain an arc so that the program can calculate the proper center point to drill or to calculate the diameter if 2 Axis Hole Pocketing or Hole Profiling is used. Partial holes can also be machined using a standard 2 Axis Profiling toolpath strategy.

 

 

For more information:

Here is the list of articles in this series: 

1. Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
2. Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
3. Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
4. Hole Machining in 2 & 3 Axis CAM Part 4: Output Control

The Bicycle Helmet Project at IYRS

Kelsey Britton is the Composites Technology program manager and instructor at IYRS School of Technology & Trades in Newport, RI. We recently sat down with Kelsey to discuss her use of RhinoCAM as part of the curriculum in her Composites Technology class. Kelsey says that she uses many of the articles on the MecSoft Tech Blog to learn and teach her students how to be proficient in RhinoCAM. Here is a project by IYRS student Wyatt Jeffries recently completed in Kelsey’s class with the help of RhinoCAM.

The Bicycle Helmet Project

In this project, Wyatt manufactures a bicycle helmet using composite technology materials and techniques. The helmet design was loaded into Rhino 3D where the surfaces were used to design mold cavities. The mold was then used to create the composite fiberglass lay-up of the outer shell. It was also used as a fixture to machine the helmet’s foam inserts. The 3D model of the helmet is shown in Rhino below.

 

 

“We chose to teach Rhino 3D to our students because of its dominance in the marine industry. RhinoCAM was a natural extension of that decision and honestly I love our RhinoCAM! I like the fact that its surface based. I can do just about anything with it. Also, the articles on the MecSoft Blog have been very helpful for setting up my curriculum. Every semester I feel that MecSoft supplies more ways to access support and that is huge for me.” Kelsey Britton, Program Manager & Instructor IYRS School of Technology & Trades, Newport, RI

For this project right and left mold halves of the outer helmet shell were designed in Rhino using surfaces extracted from the original 3D CAD model. Only the outer shell needs to be represented by the cavity. Shown below is the right side mold cavity block. After the cavity block design is completed, RhinoCAM is used to create the toolpath strategies and the G-Code needed for the Fagor 8055 controller on the school’s Freedom Patriot 3 Axis CNC router.

In the left side image below we see the right half cavity mold. The four locators indicate which face is mated with the left side cavity. In the right side image we see a 2½ Axis Facing operation to level the parting plane and a 3 Axis pocketing operation for the four locators.

(Left) The Rhino model of the left side cavity block mold is shown. (Right) We see the cavity block cut material simulation and in-process stock displayed in RhinoCAM. The parting plane and 4 locators are shown.

 

Machining the Cavities with RhinoCAM

In the left side image below we see the cut material simulation and in-process stock results of a 3 Axis Horizontal Roughing toolpath strategy also referred to as Z-Level Roughing. Using a 12.7 mm diameter flat end millI, this strategy is used to clear out material from the cavity. Cutting parameters include a 0.6 mm stock allowance, an Offset cut pattern and a Mixed cut direction. The cutting tool works its way out from the center of the cavity at a 40% stepover distance. Each cut level begins with a 10 degree path entry and removes material at a depth of 50% of the cutting tool diameter. Arc fitting in each XY plane is also performed to maximize surface finish and accuracy.

 

(Top Left) We see the cavity cut material simulation and in-process stock from the 3 Axis Horizontal Z-Level Roughing operation. (Top Right) We see the completed cut material simulation and in-process stock from the 3 Axis Horizontal Z-Level Finishing operation.

In the right side image above we see the results of a 3 Axis Horizontal Finishing toolpath strategy using a 6.35 mm diameter ball mill. This toolpath strategy is also referred to as Z-Level finishing. Cut parameters include a Stock Allowance of zero, a Climb cut direction and a Stepdown of 1 mm between Z levels. In this strategy the steep side areas of the cavity are cut with the radius and sides of the tool. In the flatter areas, optimized machining is enabled which adds additional cutting paths utilizing the tip of the ball mill, all in one toolpath.

Production

Each cavity block is made up of 6 levels of 10 mm thick MDF. The machined cavities are then visually checked, hand sanded where needed and the right and left halves are clamped together using the locators for alignment. To prepare the cavity for composite layup, 4-5 coats of epoxy resin are applied, then up to 600 grit sanding, buffing and polishing. The completed cavity is shown in the left side image below. On the right we see the fiberglass composite material placed into the cavity. The same cavity mold is also used as a fixture to machine the inner foam inserts of the helmet!

 

(Top Left) The completed and assembled right and left side cavities, coated, sanded and polished. (Top Right) The composite fiberglass lay-up of the helmet outer shell.

 

(Top Left) Wyatt gives the mold cavities some last minute preparation. (Top Right) The final composite helmet and foam insert assembly.

— Great job Wyatt! —

 

More about IYRS

IYRS School of Technology & Trades, located in Newport, Rhode Island offers marine industry classes on Composites Technology, Marine Systems, Boatbuilding & Restoration as well as Digital Modeling & Fabrication. To learn more about the IYRS programs we invite you to visit them online at iyrs.edu as well as on Facebook, Twitter and Instagram.