Rules when a Similarity of Hole Z Depths are encountered during AFM |
|
Variation
|
Conditions & Rules
|

|
Condition: Start Z position is at start of a segment. Z Depth spans an entire section.
|
Rule: Map start Z position to start of similar segment. Map Z depth to the entire depth of similar segment.
|

|
Condition: Start Z position is at start of a segment. Z Depth spans multiple sections.
|
Rule: Map start Z position to start of similar segment. Map Z depth to span all similar segments.
|

|
Condition: Start Z position is at start of a segment. Z Depth is smaller than the same segment height.
|
Rule: Map start Z position to start of similar segment. Map Z depth to a value computed as a ratio of the Z heights of the similar segments.
|

|
Condition: End Z position is at end of a segment. Z Depth is smaller than the same segment height.
|
Rule: Map end Z position to end of similar segment. Map Z depth to a value computed as a ratio of the Z heights of the similar segments.
|

|
Condition: Both Start and End Z positions are between the start and end of a segment.
|
Rule: Map start and end Z positions to values computed as a ratio of the Z heights of the similar segments.
|

|
Condition: Start Z position is at start of a segment. End Z position is between another segment.
|
Rule: Map start Z position to start of similar segment.
Map end Z position to a value computed as a ratio of the Z heights of the similar segments where the Z height ends.
Make sure all completely spanned segments between the start and end Z are also completely spanned.
|

|
Condition: Start Z position is between a segment. End Z position is at the end of a segment.
|
Rule: Map start Z position to a value computed as a ratio of the Z heights of the similar segments where the Z height starts.
Map end Z position to end of similar segment.
Make sure all completely spanned segments between the start and end Z are also completely spanned.
|

|
Condition: Start Z position is between a segment. End Z position is also between a segment.
|
Rule: Map start Z position to a value computed as a ratio of the Z heights of the similar segments where the Z height starts.
Map end Z position to a value computed as a ratio of the Z heights of the similar segments where the Z height ends.
Make sure all completely spanned segments between the start and end Z are also completely spanned.
|

|
Condition: Completely dissimilar holes are found.
|
Rule: The system will ignore the operations and have a status message (or error message) stating that some KB operations were not applied.
|
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 Features Information Dialog
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.

Detected Features List
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.

Right-click Feature Machining Context Menu (from Features List)
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.

Right-click Feature Machining Context Menu (from Part)
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.

CAM Preferences > Features
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.

Set CAM System Preferences menu item
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.

CAM Preferences > Features
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.

Right-click Feature Machining Context Menu (from Part)
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.

CAM Preferences > Features
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.

Select/Load/Create Operations for Machining Hole Features Dialog
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:
- Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
- Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
- Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
- Hole Machining in 2 & 3 Axis CAM Part 4: Output Control
May 28, 2019
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 2 of our series we explore the Hole Cutting Parameters available to each hole operation. You will learn about each hole type’s canned cycle code properties and the Cut Parameters of two 2 Axis Milling toolpath strategies that are used exclusively for cutting holes. These are 2 Axis Hole Pocketing and 2 Axis Hole Profiling. Hole Sorting Rules are also included in this section.
The following 4 blog articles are included in this series:
- Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
- Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
- Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
- Hole Machining in 2 & 3 Axis CAM Part 4: Output Control
Hole Machining Parameters
Each hole operation dialog has a Cut Parameters tab that contains all of the cycle parameters needed to define the hole. For example the Drill operation dialog includes a Drill Type selection menu that allows you to define the type of drill cycle to define. For drilling, the menu includes Standard Drill, Deep Drill, Break Chip Drill, Countersink Drill as well as four User Defined Drill Cycles. The Canned Cycle Parameters and the Hole Milling parameters are discussed in a separate section below.
 |
 |
 |
Standard Drill |
Deep & Peck Drill |
Countersink Drill |
The tables below list the canned cycle parameters supported by each hole type. You will notice that some parameters enable or disable other parameters. For example, in the Countersink Drill type, Countersink Diameter is enabled and Depth is disabled.
Drill Cycle Cut Parameters
Example G-Codes:
G81X1.2374Y1.2374Z-0.6443R0.25F10.
G82P0X1.2374Y1.2374Z-0.1443R0.25F10.
G83X1.2374Y1.2374Z-0.6443R0.25Q0.1F10.
G73X1.2374Y1.2374Z-0.6443R0.25F10.Q0.1
Drill Cycle Cut Parameters |
Parameter |
Standard G81 |
Deep G83 |
Countersink G82 |
Breakchip G73 |
User Defined |
Depth |
 |
 |
– |
 |
 |
Add Tool Tip to Depth |
 |
 |
 |
 |
 |
Location At Top |
 |
 |
 |
 |
 |
Location At Bottom |
 |
 |
 |
 |
 |
Location Pick Top |
 |
 |
 |
 |
 |
Projects to 3D Model |
 |
 |
 |
 |
 |
Dwell Off |
 |
 |
 |
 |
 |
Dwell Time/sec |
 |
 |
 |
 |
 |
Dwell Rev/rpm |
 |
 |
 |
 |
 |
Approach Distance (R) |
 |
 |
 |
 |
 |
Countersink Diameter |
– |
– |
 |
– |
– |
Step Increment (Q) |
– |
 |
– |
 |
 |
Tap Cycle Cut Parameters
Example G-Codes:
G84X1.2374Y1.2374Z-0.5R0.1F300.
G84X1.2374Y1.2374Z-0.5R0.1Q0.1F14.667
Tap Cycle Cut Parameters |
Parameter |
Standard Tap G84 |
Peck Tap G84 |
User Defined Tap |
Depth |
 |
 |
 |
Location At Top |
 |
 |
 |
Location At Bottom |
 |
 |
 |
Location Pick Top |
 |
 |
 |
Projects to 3D Model |
 |
 |
 |
Dwell Off |
 |
 |
 |
Dwell Time/sec |
 |
 |
 |
Dwell Rev/rpm |
 |
 |
 |
Approach Distance (R) |
 |
 |
 |
Direction Right/Left |
 |
 |
 |
Cut Peck Depth (Q) |
– |
 |
– |
Bore Cycle Cut Parameters
Example G-Codes:
G85X1.2374Y1.2374Z-0.5R0.1F14.667
G86X0.750Y-0.750Z-0.500R0.100F14.7
G87X0.750Y0.750Z-0.500R0.100F14.7
Tap Cycle Cut Parameters |
Parameter |
Drag Bore G85 |
NoDrag Bore G86 |
Manual Bore G87 |
User Defined Bore |
Depth |
 |
 |
 |
 |
Location At Top |
 |
 |
 |
 |
Location At Bottom |
 |
 |
 |
 |
Location Pick Top |
 |
 |
 |
 |
Projects to 3D Model |
 |
 |
 |
 |
Dwell Off |
 |
 |
 |
 |
Dwell Time/sec |
 |
 |
 |
 |
Dwell Rev/rpm |
 |
 |
 |
 |
Approach Distance (R) |
 |
 |
 |
 |
Tool Orientation |
– |
 |
– |
 |
Reverse Bore Cycle Cut Parameters
Example G-Codes:
G77X1.2374Y1.2374Z-0.5R0.1F14.667
Tap Cycle Cut Parameters |
Parameter |
Reverse Bore G77 |
User Defined Reverse Bore |
Depth |
 |
 |
Location At Top |
 |
 |
Location At Bottom |
 |
 |
Location Pick Top |
 |
 |
Projects to 3D Model |
 |
 |
Dwell Off |
 |
 |
Dwell Time/sec |
 |
 |
Dwell Rev/rpm |
 |
 |
Approach Distance (R) |
 |
 |
Tool Orientation |
 |
 |
Hole Milling Operations
For larger holes you can select from one of the 2 Axis Milling toolpath strategies that are specifically designed for cutting circular holes and pockets using mill cutting tools. These include 2 Axis Hole Pocketing, 2 Axis Hole Profiling. It should be noted here that these are not canned holes cycles. They are 2 Axis mill cutting paths that output Linear, Arc and Helix motions. Hole Pocketing combines a helical entry motion with a spiral cut motion at each cut level. Hole Profiling is a helical cut motion combined with entry and exit motion.
 Hole Pocketing Example |
 Hole Profiling Example |
Hole Milling Cut Parameters
In addition to the Location of Cut Geometry parameters, additional Cut Parameters include a global Tolerance (t), Hole Depth (H), Hole Diameter (D), Cut Direction and Helical Pitch. Hole Pocketing also includes Stepdown (Dz), Stepover (S) and the ability to add a Cleanup Pass at each cut level. Both of these operations allow you to optionally create full 360 degree helical motions and output each helix individually in the posted G-Code. The cut parameters for each operation type are listed below.
 Hole Pocketing Cut Parameters |
 Hole Pocketing Cut Parameters |
Hole Pocketing/Profiling Cut Parameters |
Parameter |
Hole Pocketing |
Hole Profiling |
Tolerance (t) |
 |
 |
Location At Top |
 |
 |
Location At Bottom |
 |
 |
Location Pick Top |
 |
 |
Hole Depth (H) |
 |
 |
Depth from 3D Model |
 |
 |
Hole Diameter (D) |
 |
 |
Use Arc Diameter |
 |
 |
Cut Direction |
 |
 |
Stepdown (Dz) |
 |
 |
Stepover (S) |
 |
– |
Do Cleanup Pass |
 |
– |
Helical Entry |
 |
– |
Linear Entry |
– |
 |
Radial Entry |
– |
 |
Ramp Entry |
– |
 |
Full 360 Degree Helix |
 |
– |
Output each Helix Individually |
 |
– |
Hole Sorting Rules
If you have many holes to machine in one operation, you can take advantage of the Sorting tab on each hole operation dialog. It allows you to perform a Minimum Distance Sort and Directional Sort of the holes. In Minimum Distance Sort you can specify the starting location such as Lower Left, Upper Right, etc. The program will calculate the hole machining sequence based on the distance between holes.
If you have a lot of holes in a close pattern this option will keep the machining time to a minimum. If you have a lot of holes in multiple patterns you can use the Direction Sort option. This allows you to specify a Primary and Secondary Direction as well as the Traversal Pattern (i.e., Zig or ZigZag). The Sort tab is also available all Hole operation dialogs as well as many other Milling operations.

Hole Sorting Rules tab (No Sort Selected)

No Sorting Selection from Sorting Tab

Hole Sorting Rules tab (Minimum Distance Selected)

Minimum Distance / Upper Left Selected from the Sorting Tab

Hole Sorting Rules tab (Direction Selected)

Directional Sort, High to Low, ZigZag Selected from the Sorting Tab
For more information:
Here is the list of articles in this series:
- Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
- Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
- Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
- Hole Machining in 2 & 3 Axis CAM Part 4: Output Control
May 24, 2019
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:
- Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
- Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
- Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
- 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 Holes from a 2D Drawing
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 Holes from a 3D 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.

Selecting Holes from a 3D Solid Model with Hole Features

Selecting Holes from the Feature Tree
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.

Selecting Holes on Flat Areas
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.

The Diameter Range Filter

The Diameter Range Filter
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.

Locating the Machining Objects Browser Toggle

The Regions Tab
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.

Specify Flat Areas Selections Filter
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.

Flat Area Selected
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.

Holes on Flat Area are Filtered and Selected

Flat Area Regions (i.e., each Hole) is Listed in a Machining Region Set
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.

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

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

PreDefined Regions are added to the Hole Features tab
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.

Machining Partial Holes for 2 Axis Hole Profiling
For more information:
Here is the list of articles in this series:
- Hole Machining in 2 & 3 Axis CAM Part 1: Geometry Selections
- Hole Machining in 2 & 3 Axis CAM Part 2: Cutting Parameters
- Hole Machining in 2 & 3 Axis CAM Part 3: Program Automation
- Hole Machining in 2 & 3 Axis CAM Part 4: Output Control
May 14, 2019

IYRS School of Technology & Trades is a non-profit, post-secondary experiential learning school located in Newport, Rhode Island. The school offers education & training programs for craftspeople, artists, fixers, technicians, thinkers, problem-solvers, and creatives! Set on Aquidneck Island, Newport and its yacht-filled harbor hosted the America’s Cup, a renowned annual sailing regatta, for many years. The school’s alumni are rapidly employed into the local shipbuilding industry which helps makes Newport one the most popular lifestyle and tourist destinations on the New England sea coast.
Be sure to check out the video below of IYRS alumni help to restore The Mayflower II at Mystic Seaport in Mystic, CT.
IYRS School of Technology & Trades was originally founded on the boatbuilding restoration program. A 20-month program to master the craft and fundamentals of restoring, building, and finishing classic wooden yachts. Students build a beetle cat sailboat the first year and then come back the second year and learn boat building restoration. The school has recently added three additional programs, Composites Technology, Marine Systems, and Digital Modeling & Fabrication.
Composites Technology
Kelsey Britton is the Composites Technology program manager and instructor at IYRS School of Technology & Trades and considers shipbuilding to be more a way of life than a job! Her mother taught Kelsey how to sail as a child. Her brother is a ferry boat captain in New London, CT and her father is a career marine mechanic and manager. Kelsey started her career in hospitality, doing everything from bussing tables to managing entire restaurants. Soon however, the love of the boat building trade urged her back home where she enrolled and excelled in the school’s yacht restoration program. Kelsey made such a positive impression on the staff that in no short order she was offered and accepted a full-time position to teach at the school she loves!
 |
“The marine industry and shipbuilding specifically is more a lifestyle than a job. I love what I do – teaching others how to find that passion and help them move forward in life and hopefully continue and work in the marine industry!”
Kelsey Britton, Program Manager & Instructor
IYRS School of Technology & Trades, Newport, RI |
We recently sat down with Kelsey to discuss her use of RhinoCAM as part of her 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. Kelsey likes how RhinoCAM’s user interface pop-ups helpful information about the various machining parameters and specifically mentions MecSoft’s technical support as a key part of her classes success. Here is a project that IYRS student Simon Pride recently completed in Kelsey’s class with the help of RhinoCAM.
The Marine Steering Wheel Project
In this project Simon designs and manufactures the marine steering wheel shown in Rhino below using composite technology materials and techniques. Simon used the 3D model to split and subtract a cavity to design the mold block. The design consists of the main steering wheel that is 22 mm in cross-section and 445 mm in outer diameter. The center connecting spoke is 6 mm thick and blends into the main wheel at both ends. The central parting line lies in on XY plane. The steering wheel 3D model is shown below in Rhino.

The 3D model of the steering wheel design is shown in Rhino. The transition area between the spoke and the wheel is shown enlarged so you can see the blending of surfaces that need to be incorporated into the mold cavities.
3 Axis Z-Level Roughing in RhinoCAM
In the left image below we see the bottom cavity mold half for the steering wheel. The view shows where the center spoke transitions into the outer wheel. In the right image we see the remaining cut material simulation and in-process stock left after a 3 Axis Horizontal Roughing toolpath using a 3 mm diameter end mill.
The cut parameters include a Stock Allowance of 1.259 mm, an Offset cut pattern, Mixed cut direction, an Inside start point and a 40% tool Stepover. For cut levels, a Stepdown distance of 2 mm and a maximum Top Z height of 50.8 mm. The Clear Flats option is also checked which ensures that a cleanup finish pass is located on the floor of the spoke cavity. The 1.259 mm stock allowance ensures that only the vertical side walls of the spoke need to be finished.
 |
 |
(Top Left) The 3D model of the bottom cavity mold is shown in Rhino. (Top Right) The cut material simulation showing the in-process stock after the 3 Axis Horizontal Z-Level Roughing toolpath is completed. |
3 Axis Horizontal Z-Level Finishing
For finishing the cavity, two RhinoCAM 3 Axis Horizontal Z-Level Finishing operations are performed using the same 3 mm diameter ball mill. The first finishes the outer wheel cavity and the second finishes the inner spoke cavity. A 3 Axis Pencil Trace operation is also performed using the same 3mm ball mill as a finishing pass. It calculates the bi-tangent path between the spoke floor and the drafted spoke side walls. In the right side image we see the actual mold half after being prepared for composite lay-up.
 |
 |
(Top Right) The resulting RhinoCAM cut material simulation after the 3 Axis finishing toolpaths are completed. (Top Right) The actual mold cavity after being prepped for composite layup. |
 |
 |
Student Simon Pride prepares his composite marine steering wheel for assembly. |
— Cool project Simon! —
We want to thank Kelsey Britton and IYRS School of Technology & Trades in Newport, RI for allowing us to showcase their student’s work!
IYRS Alumni Help Restore The Mayflower II
Alumni of the two-year Boatbuilding & Restoration program at IYRS School of Technology & Trades in Newport, RI are featured in this video focused on the restoration of the Mayflower II and the IYRS externship with Mystic Seaport in Mystic, CT.
https://www.youtube.com/watch?v=sBFIVuIyiWM
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.

IYRS School of Technology & Trades in Newport, RI.
May 7, 2019
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.

The 3D surface model of the bicycle helmet is shown in the Rhino 3D modeling program. The design consists of an outer shell and an inner foam insert.
 |
“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.

IYRS School of Technology & Trades in Newport, RI.
May 2, 2019
Being a new user on MecSoft’s Annual Maintenance Subscription service (AMS) you not only get annual upgrades, enhanced one-on-one support and access to our user forums. You also get exclusive access to our CAMJam Self Training library! This download includes the CAMJam Video Archive Guide, the MecSoft CAM Question & Answer Guide, The Cutting Tools Workbook, The F1 CO2 Racer Body Tutorial, the training part file archive as well as easy access to all available print materials through our new Resource Guides for each product.
Here are the basic steps to download your CAMJam Self Training materials:
1. When you sign up for AMS you will receive an email with your login credentials to the MecSoft VisualSERVE customer portal.

2. Enter the email address and password provided to you in the email. Note: Make sure you see and check the CAPTCHA to confirm that you are a real user!

3. From your MecSoft VisualSERVE Customer Portal home page, locate the Download CAMJam button and select it.

4. Download the MecSoft CAMJam archive file to your local hard drive, extract the contents and you are on your way to self-learning your MecSoft CAM plugin!
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: