& Construction
![architecture engineering and construction collection logo](https://damassets.autodesk.net/content/dam/autodesk/www/universal-header/flyout/architecture-engineering-construction-collection-uhblack-banner-lockup-364x40.png)
Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing
![product design manufacturing collection logo](https://damassets.autodesk.net/content/dam/autodesk/www/universal-header/flyout/product-design-manufacturing-collection-uhblack-banner-lockup-364x40.png)
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
Learn about what happens when a tool orientation is selected and the effect on the toolpath.
Type:
Tutorial
Length:
7 min.
Transcript
00:03
Making selections to define tool orientation on a model is simple and straightforward if there are a lot of flat faces and straight edges.
00:12
But that is not always the case, as with this hockey scale adapter that was designed for a player with a leg length discrepancy.
00:19
This adapter is made up of mostly non-planar surfaces and complex edges,
00:24
rather than planar faces and straight edges, which will present more of a challenge when making selections.
00:30
To start, focus on the top front truck.
00:33
In the Browser, hide any visible parts other than the Top Front truck.
00:38
Switch to the Manufacture workspace.
00:41
Note that one side is already roughed out, and the horizontal face on the flange is complete.
00:47
Now, you will finish the rest of this side, which is largely non-planar surfaces, with two planar faces at odd angles.
00:55
Based on the upper angled face and fillet, it looks as if a parallel operation would work well.
01:00
First, expand the setups and activate Side1.
01:04
From the Milling toolbar, 3D group, click Parallel.
01:10
In the Parallel dialog, Tool tab, click Select.
01:15
In the Select Tool dialog, make sure that the current design is selected under Documents,
01:20
select the 1/8-inch ball end mill tool, and then click Select.
01:26
Switch to the Geometry tab and start with defining a machining boundary.
01:31
It also looks like you will need to set the Tool Orientation to avoid colliding with the flange.
01:36
Notice however, that none of the geometry lends itself nicely to defining the Z axis for this operation.
01:43
You can try using the angled face on the other side of the part, but that does not give you much control over the tool path,
01:50
as it is not a great angle for the tool.
01:53
Instead of using part geometry to define the Z, you can create and use work geometry.
01:59
Cancel the Parallel operation.
02:02
Switching to the Design workspace, activate the top front truck, so that all the geometry you create is stored within that component.
02:10
On the Solid toolbar, in the Construct menu, there are options to create planes, axes, and points.
02:18
Select Plane Through Two Edges, and then choose the edges on either side of the radius.
02:25
Fusion gives you an error, because lines must intersect or be parallel.
02:29
Even though these are straight edges, they cannot generate a work plane.
02:34
Expand the Construct menu again and select Plane Through Three Points instead.
02:39
Select three points along the perimeter of the inside fillet on the geometry to generate a plane angled in the direction you want.
02:47
While this looks good, you can create another plane, just in case a different angle is needed.
02:53
From the Construct menu, select Plane at Angle.
02:57
Select the straight edge on the inside of the angled planar face, then use the angle slider to approximate the angle of the plane.
03:05
If you have a specific angle you want to use for the plane, you can enter it directly.
03:10
Note that the plane will lie along the selected edge, so if you do not like how the plane is aligned, you can select another edge instead.
03:19
Now that you have a few work planes to use, switch back to the Manufacture workspace, and from the 3D group, click Parallel.
03:27
In the Parallel dialog, Tool tab, click Select to open the Select Tool dialog, choose the 1/8-inch Ball end mill tool, and then click Select.
03:38
On the Geometry tab, set the Machining Boundary to Selection.
03:44
Select the flat face and the fillet that define the area to be machined.
03:48
Change to the Multi-Axis tab and check Tool Orientation.
03:53
In the Browser, expand Model then expand the 3_Tool Orientation Definition, Top Front Truck, Construction.
04:05
Select the first of the two new work planes to define the Z axis.
04:09
Zooming out a little, you can see the direction Z is facing with relationship to the plane Z,
04:15
depending on how the 3-point plane was created.
04:19
When using work planes or edges, Fusion does not always know where the part geometry is.
04:24
If the Z axis is pointing towards the bottom, you can use the arrow tip or select Flip Z Axis in the dialog to point it in the correct direction.
04:35
You do not need to define an X or Y direction, since this is handled when the code gets posted.
04:40
The post-processor knows the direction that Z needs to point and then finds an X and Y that the machine is capable of.
04:48
However, there is a parameter within the toolpath that is driven off the X axis pass direction,
04:54
and based on the current X direction, the parallel passes are not going to be great for the geometry.
05:00
On the Passes tab, you can adjust the Pass Direction.
05:05
However, if you do not know exactly what the optimal angle will be,
05:09
you can control the passes by redefining the X axis in the direction you would like the passes to go.
05:15
Click OK to generate the toolpath.
05:18
In the Browser, right-click the Parallel operation you just created and select Duplicate.
05:23
Right-click the new operation and select Edit.
05:27
In the Parallel dialog, Multi-Axis tab, click the X to remove the Z Axis selection.
05:35
Then, select the other work plane as the Z axis.
05:39
Again, zoom out and check to see if you need to flip the Z axis.
05:43
If needed, select Flip Z Axis.
05:46
Also, make sure the X direction is the same as the previous operation, so the passes point in that direction.
05:53
Click OK to generate the toolpath.
05:56
To compare the toolpaths, from the Navigation bar, click the Constrained Orbit tool,
06:02
then rotate the view so that you can see the toolpath and the tool as vertical.
06:07
Using this configuration, it looks like the first Parallel toolpath gives slightly more clearance and blends a little better with the flat face.
06:16
One other use for work geometry and 3+2 toolpaths is using tilting
06:22
to avoid cutting along the center line of a ball end mill when running finishing passes.
06:27
Since the center of the tool technically has a radius of 0,
06:31
the surface speed near the center is always near 0, which leads to reduced tool life and poor surface finish.
06:37
You can apply this principle to finish the top surface of the top front truck.
06:49
Switch back to the Design workspace.
06:52
In the Browser, hide the two visible work planes.
06:55
Then, orbit the view so that you can see the top of the truck.
06:59
From the Construct menu, select Plane at Angle, and then select the Z axis.
07:07
Set the angle to 20 degrees.
07:10
Change back to the Manufacture workspace.
07:14
In the Browser, activate the Top Front 2 Back operation.
07:18
Orbit the view so that you can see the top of the part, which in this case, is the bottom view.
07:24
Next, from the 3D group, select Parallel to finish the surface.
07:30
In the Parallel dialog, Tool tab, click Select.
07:35
In the Select Tool dialog, browser, be sure the current document is selected, and choose the 1/8-inch ball end mill, then click Select.
07:45
Change to the Geometry tab, set the Machine Boundary to Selection, then select the upper face.
07:54
In the Multi-Axis tab, select Tool Orientation, and then select the plane you just created.
08:03
The tool is now running with side tilt, or along the axis that the tilt is happening around.
08:09
Click OK to generate the toolpath.
08:12
The resulting toolpath keeps the tool engaged up the radius away from the center line of the tool.
08:18
In addition to using work geometry to help with multi-axis toolpath definitions,
08:23
you can also use sketch geometry on the work plane to contain the toolpath.
08:28
For example, you can use a sketched rectangle that approximately contains the geometry you want to finish.
08:34
Then, while creating the Parallel operation, you can select the sketch geometry as the machining boundary.
08:41
This can help when geometry is difficult to select,
08:44
or if the projection onto the selected tool orientation coordinate system does not generate the toolpath as expected.
08:51
The post processor takes care of the X and Y orientation calculations,
08:56
so that all you need to do is define the correct Z axis and make sure the pass direction is appropriate.
Video transcript
00:03
Making selections to define tool orientation on a model is simple and straightforward if there are a lot of flat faces and straight edges.
00:12
But that is not always the case, as with this hockey scale adapter that was designed for a player with a leg length discrepancy.
00:19
This adapter is made up of mostly non-planar surfaces and complex edges,
00:24
rather than planar faces and straight edges, which will present more of a challenge when making selections.
00:30
To start, focus on the top front truck.
00:33
In the Browser, hide any visible parts other than the Top Front truck.
00:38
Switch to the Manufacture workspace.
00:41
Note that one side is already roughed out, and the horizontal face on the flange is complete.
00:47
Now, you will finish the rest of this side, which is largely non-planar surfaces, with two planar faces at odd angles.
00:55
Based on the upper angled face and fillet, it looks as if a parallel operation would work well.
01:00
First, expand the setups and activate Side1.
01:04
From the Milling toolbar, 3D group, click Parallel.
01:10
In the Parallel dialog, Tool tab, click Select.
01:15
In the Select Tool dialog, make sure that the current design is selected under Documents,
01:20
select the 1/8-inch ball end mill tool, and then click Select.
01:26
Switch to the Geometry tab and start with defining a machining boundary.
01:31
It also looks like you will need to set the Tool Orientation to avoid colliding with the flange.
01:36
Notice however, that none of the geometry lends itself nicely to defining the Z axis for this operation.
01:43
You can try using the angled face on the other side of the part, but that does not give you much control over the tool path,
01:50
as it is not a great angle for the tool.
01:53
Instead of using part geometry to define the Z, you can create and use work geometry.
01:59
Cancel the Parallel operation.
02:02
Switching to the Design workspace, activate the top front truck, so that all the geometry you create is stored within that component.
02:10
On the Solid toolbar, in the Construct menu, there are options to create planes, axes, and points.
02:18
Select Plane Through Two Edges, and then choose the edges on either side of the radius.
02:25
Fusion gives you an error, because lines must intersect or be parallel.
02:29
Even though these are straight edges, they cannot generate a work plane.
02:34
Expand the Construct menu again and select Plane Through Three Points instead.
02:39
Select three points along the perimeter of the inside fillet on the geometry to generate a plane angled in the direction you want.
02:47
While this looks good, you can create another plane, just in case a different angle is needed.
02:53
From the Construct menu, select Plane at Angle.
02:57
Select the straight edge on the inside of the angled planar face, then use the angle slider to approximate the angle of the plane.
03:05
If you have a specific angle you want to use for the plane, you can enter it directly.
03:10
Note that the plane will lie along the selected edge, so if you do not like how the plane is aligned, you can select another edge instead.
03:19
Now that you have a few work planes to use, switch back to the Manufacture workspace, and from the 3D group, click Parallel.
03:27
In the Parallel dialog, Tool tab, click Select to open the Select Tool dialog, choose the 1/8-inch Ball end mill tool, and then click Select.
03:38
On the Geometry tab, set the Machining Boundary to Selection.
03:44
Select the flat face and the fillet that define the area to be machined.
03:48
Change to the Multi-Axis tab and check Tool Orientation.
03:53
In the Browser, expand Model then expand the 3_Tool Orientation Definition, Top Front Truck, Construction.
04:05
Select the first of the two new work planes to define the Z axis.
04:09
Zooming out a little, you can see the direction Z is facing with relationship to the plane Z,
04:15
depending on how the 3-point plane was created.
04:19
When using work planes or edges, Fusion does not always know where the part geometry is.
04:24
If the Z axis is pointing towards the bottom, you can use the arrow tip or select Flip Z Axis in the dialog to point it in the correct direction.
04:35
You do not need to define an X or Y direction, since this is handled when the code gets posted.
04:40
The post-processor knows the direction that Z needs to point and then finds an X and Y that the machine is capable of.
04:48
However, there is a parameter within the toolpath that is driven off the X axis pass direction,
04:54
and based on the current X direction, the parallel passes are not going to be great for the geometry.
05:00
On the Passes tab, you can adjust the Pass Direction.
05:05
However, if you do not know exactly what the optimal angle will be,
05:09
you can control the passes by redefining the X axis in the direction you would like the passes to go.
05:15
Click OK to generate the toolpath.
05:18
In the Browser, right-click the Parallel operation you just created and select Duplicate.
05:23
Right-click the new operation and select Edit.
05:27
In the Parallel dialog, Multi-Axis tab, click the X to remove the Z Axis selection.
05:35
Then, select the other work plane as the Z axis.
05:39
Again, zoom out and check to see if you need to flip the Z axis.
05:43
If needed, select Flip Z Axis.
05:46
Also, make sure the X direction is the same as the previous operation, so the passes point in that direction.
05:53
Click OK to generate the toolpath.
05:56
To compare the toolpaths, from the Navigation bar, click the Constrained Orbit tool,
06:02
then rotate the view so that you can see the toolpath and the tool as vertical.
06:07
Using this configuration, it looks like the first Parallel toolpath gives slightly more clearance and blends a little better with the flat face.
06:16
One other use for work geometry and 3+2 toolpaths is using tilting
06:22
to avoid cutting along the center line of a ball end mill when running finishing passes.
06:27
Since the center of the tool technically has a radius of 0,
06:31
the surface speed near the center is always near 0, which leads to reduced tool life and poor surface finish.
06:37
You can apply this principle to finish the top surface of the top front truck.
06:49
Switch back to the Design workspace.
06:52
In the Browser, hide the two visible work planes.
06:55
Then, orbit the view so that you can see the top of the truck.
06:59
From the Construct menu, select Plane at Angle, and then select the Z axis.
07:07
Set the angle to 20 degrees.
07:10
Change back to the Manufacture workspace.
07:14
In the Browser, activate the Top Front 2 Back operation.
07:18
Orbit the view so that you can see the top of the part, which in this case, is the bottom view.
07:24
Next, from the 3D group, select Parallel to finish the surface.
07:30
In the Parallel dialog, Tool tab, click Select.
07:35
In the Select Tool dialog, browser, be sure the current document is selected, and choose the 1/8-inch ball end mill, then click Select.
07:45
Change to the Geometry tab, set the Machine Boundary to Selection, then select the upper face.
07:54
In the Multi-Axis tab, select Tool Orientation, and then select the plane you just created.
08:03
The tool is now running with side tilt, or along the axis that the tilt is happening around.
08:09
Click OK to generate the toolpath.
08:12
The resulting toolpath keeps the tool engaged up the radius away from the center line of the tool.
08:18
In addition to using work geometry to help with multi-axis toolpath definitions,
08:23
you can also use sketch geometry on the work plane to contain the toolpath.
08:28
For example, you can use a sketched rectangle that approximately contains the geometry you want to finish.
08:34
Then, while creating the Parallel operation, you can select the sketch geometry as the machining boundary.
08:41
This can help when geometry is difficult to select,
08:44
or if the projection onto the selected tool orientation coordinate system does not generate the toolpath as expected.
08:51
The post processor takes care of the X and Y orientation calculations,
08:56
so that all you need to do is define the correct Z axis and make sure the pass direction is appropriate.
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.