& Construction

Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing

Professional CAD/CAM tools built on Inventor and AutoCAD
Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Finish Contour toolpaths. Covers multiple cuts, cutter compensation and lead in/lead out.
Type:
Tutorial
Length:
7 min.
Transcript
00:03
In Fusion, 2D Contour milling creates a toolpath based on a contour selection, which is an outline of a part.
00:11
You can select a sketch or an edge on the part for the contour selection.
00:16
The contour selections can be open chains or closed chains and can be on the inside or outside of a part.
00:24
In 2D Contour, the cutting motion always takes place on a 2D plane.
00:35
You can use multiple finishing passes to avoid cutting with the full width of the cutter.
00:41
You can also machine tabs to help hold a part in place, which is useful when cutting on a sheet of material.
00:48
In this example, you want to create the finish cuts on the outer profile, the open pockets, and the closed pockets.
00:57
A single 2D contour toolpath can contain multiple chains,
01:02
and each can be cut to its own specific depth, if the cutting parameters are the same.
01:07
This means that they will use the same feed speed and number of cuts.
01:13
In the Manufacture workspace, Milling toolbar, 2D group, select 2D Contour.
01:20
In the example part, the smallest inside radius is 150 thousandths.
01:27
Therefore, you need to select a tool that fits within this parameter.
01:32
From the 2D Contour dialog, Tool tab, click Select to open the Tool Library, where you can select your cutting tool.
01:41
For this example, under Document, click Intro to 2D Machining to show only the tools for this project.
01:49
Select tool 3 (1/4” Flat End Mill) from the list, and then click Select.
01:56
In the 2D Contour dialog, the default Speeds & Feeds for this tool are acceptable, so you can switch to the Geometry tab.
02:05
Keep in mind, there are many areas on this part that require a finished contouring toolpath.
02:12
When selecting the geometry, only choose multiple contours if they have similar cutting attributes.
02:19
You want to cut around the outside of the part.
02:22
However, do not cut past the bottom edge on the pockets, as that would ruin the part.
02:28
For the initial toolpath, click Select, and then click the bottom edge.
02:34
Next, switch to the Heights tab.
02:37
Set the Bottom Height to From Selected contour(s), and the Offset depth to -.03 inches, so you cut past the bottom edge of the part.
02:47
Switch to the Passes tab.
02:50
The 2D contour toolpath is almost always used as a finishing cut.
02:56
This means that you need to hold the final size, based on the tolerance and the part requirements.
03:02
While Fusion will calculate the toolpath to the highest resolution that the machine can accept,
03:08
there are factors that can make holding that tolerance difficult during the machining process.
03:14
Tool wear is the biggest problem in controlling the tolerance at the machine tool.
03:19
Providing the CNC machine operator some control over the final size of the cut is necessary.
03:26
This is done with cutter diameter compensation, sometimes referred to as cutter radius compensation, or more commonly, cutter comp.
03:35
To provide the CNC operator with the control needed, use the Compensation Type setting.
03:42
Read the tooltip to see what each of these options will do.
03:46
To enable cutter comp at the machine, set the Compensation Type to either Wear or Inverse wear.
03:53
This will output the code to provide compensation to the left or to the right of the programmed path.
03:60
The actual code will depend on the specific CNC machine control requirements.
04:06
The most common codes are G41, which is cutter comp left, and G42, which is cutter comp right.
04:14
For this example part, set the Compensation Type to Wear.
04:19
Other parameters that you may find useful on this tab are in the Roughing Passes and Multiple Depths groups.
04:27
Roughing passes take additional side cuts on the part.
04:31
Multiple depths take multiple steps going down in Z.
04:36
For now, leave these off, but consider looking at the tooltips and trying those options later.
04:43
Select the checkbox next to Smoothing.
04:46
Switch to the Linking tab.
04:49
You never want to drop your tool right on the edge of the part.
04:53
To avoid this, use the Leads & Transitions settings.
04:58
Lead-in blends onto the part and Lead-out blends off the part.
05:03
These parameters create a series of arc and line moves for a smooth transition onto the cut.
05:10
Examine the tooltips for details on what the individual parameters are controlling.
05:16
For now, leave these set to their defaults.
05:20
These values are set by a formula based on the tool size.
05:25
If you want to investigate, click the More menu for these settings, and select Edit Expression to see the formula for each.
05:34
Typically, you would want the Lead-out to be the same as the Lead-in.
05:38
However, you can disable Same as Lead-in and make your Lead-out a completely different set of values.
05:46
Click OK to generate a toolpath around the outside of the part.
05:51
Save your model if you want to continue working on it.
Video transcript
00:03
In Fusion, 2D Contour milling creates a toolpath based on a contour selection, which is an outline of a part.
00:11
You can select a sketch or an edge on the part for the contour selection.
00:16
The contour selections can be open chains or closed chains and can be on the inside or outside of a part.
00:24
In 2D Contour, the cutting motion always takes place on a 2D plane.
00:35
You can use multiple finishing passes to avoid cutting with the full width of the cutter.
00:41
You can also machine tabs to help hold a part in place, which is useful when cutting on a sheet of material.
00:48
In this example, you want to create the finish cuts on the outer profile, the open pockets, and the closed pockets.
00:57
A single 2D contour toolpath can contain multiple chains,
01:02
and each can be cut to its own specific depth, if the cutting parameters are the same.
01:07
This means that they will use the same feed speed and number of cuts.
01:13
In the Manufacture workspace, Milling toolbar, 2D group, select 2D Contour.
01:20
In the example part, the smallest inside radius is 150 thousandths.
01:27
Therefore, you need to select a tool that fits within this parameter.
01:32
From the 2D Contour dialog, Tool tab, click Select to open the Tool Library, where you can select your cutting tool.
01:41
For this example, under Document, click Intro to 2D Machining to show only the tools for this project.
01:49
Select tool 3 (1/4” Flat End Mill) from the list, and then click Select.
01:56
In the 2D Contour dialog, the default Speeds & Feeds for this tool are acceptable, so you can switch to the Geometry tab.
02:05
Keep in mind, there are many areas on this part that require a finished contouring toolpath.
02:12
When selecting the geometry, only choose multiple contours if they have similar cutting attributes.
02:19
You want to cut around the outside of the part.
02:22
However, do not cut past the bottom edge on the pockets, as that would ruin the part.
02:28
For the initial toolpath, click Select, and then click the bottom edge.
02:34
Next, switch to the Heights tab.
02:37
Set the Bottom Height to From Selected contour(s), and the Offset depth to -.03 inches, so you cut past the bottom edge of the part.
02:47
Switch to the Passes tab.
02:50
The 2D contour toolpath is almost always used as a finishing cut.
02:56
This means that you need to hold the final size, based on the tolerance and the part requirements.
03:02
While Fusion will calculate the toolpath to the highest resolution that the machine can accept,
03:08
there are factors that can make holding that tolerance difficult during the machining process.
03:14
Tool wear is the biggest problem in controlling the tolerance at the machine tool.
03:19
Providing the CNC machine operator some control over the final size of the cut is necessary.
03:26
This is done with cutter diameter compensation, sometimes referred to as cutter radius compensation, or more commonly, cutter comp.
03:35
To provide the CNC operator with the control needed, use the Compensation Type setting.
03:42
Read the tooltip to see what each of these options will do.
03:46
To enable cutter comp at the machine, set the Compensation Type to either Wear or Inverse wear.
03:53
This will output the code to provide compensation to the left or to the right of the programmed path.
03:60
The actual code will depend on the specific CNC machine control requirements.
04:06
The most common codes are G41, which is cutter comp left, and G42, which is cutter comp right.
04:14
For this example part, set the Compensation Type to Wear.
04:19
Other parameters that you may find useful on this tab are in the Roughing Passes and Multiple Depths groups.
04:27
Roughing passes take additional side cuts on the part.
04:31
Multiple depths take multiple steps going down in Z.
04:36
For now, leave these off, but consider looking at the tooltips and trying those options later.
04:43
Select the checkbox next to Smoothing.
04:46
Switch to the Linking tab.
04:49
You never want to drop your tool right on the edge of the part.
04:53
To avoid this, use the Leads & Transitions settings.
04:58
Lead-in blends onto the part and Lead-out blends off the part.
05:03
These parameters create a series of arc and line moves for a smooth transition onto the cut.
05:10
Examine the tooltips for details on what the individual parameters are controlling.
05:16
For now, leave these set to their defaults.
05:20
These values are set by a formula based on the tool size.
05:25
If you want to investigate, click the More menu for these settings, and select Edit Expression to see the formula for each.
05:34
Typically, you would want the Lead-out to be the same as the Lead-in.
05:38
However, you can disable Same as Lead-in and make your Lead-out a completely different set of values.
05:46
Click OK to generate a toolpath around the outside of the part.
05:51
Save your model if you want to continue working on it.
Manufacture > Milling > 2D > 2D Contour
2D Contour is a toolpath to finish mill a profile at a specific level (Z Depth). These profiles can be internal or external, open or closed. You have the capability of creating multiple Z steps to cut down, or multiple side cuts on the profile. But the cutting motion always takes place on a 2D plane. A single 2D Contour toolpath can contain multiple chains and each can be cut to it's own specific depth, as long as the cutting parameters are the same (Feed, Speed, Number of cuts, etc.).
Cutter Diameter/Radius Compensation can provide the NC Machine operator some way to control the final size of the cut at the machine. Set the Compensation Type to either Wear or Inverse Wear. This will output the codes to compensate to the Left or Right of the programed path. The actual code will depend on the machines NC Code requirements. The most common codes are G41 (CC Left) and G42 (CC Right).
How to buy
Privacy | Do not sell or share my personal information | Cookie preferences | Report noncompliance | Terms of use | Legal | © 2025 Autodesk Inc. All rights reserved
Sign in for the best experience
Save your progress
Get access to courses
Receive personalized recommendations
May we collect and use your data?
Learn more about the Third Party Services we use and our Privacy Statement.May we collect and use your data to tailor your experience?
Explore the benefits of a customized experience by managing your privacy settings for this site or visit our Privacy Statement to learn more about your options.