Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Take your programming efficiency to the next level with these productivity tips, including expression, templates, patterns, and NC Programs.
Type:
Tutorial
Length:
8 min.
Transcript
00:04
Everyone wants to be more productive from the principles of lean manufacturing
00:07
to shaving seconds off machine cycle times and programming is no different.
00:11
This tutorial will cover some of the productivity tips that will
00:13
save you time when programming your parts in fusion 360.
00:17
For the first tip,
00:18
let's edit this two D contour operation that
00:21
is finishing the outer contour of this bracket
00:23
in the passes tab.
00:24
You can see that we have enabled multiple depths
00:26
to split the tool path into several step downs
00:30
while hard coding 250 that will work,
00:32
it will always be that value even if there's a change to the tool.
00:35
So instead of simply typing in a value to the step down,
00:38
I can right click and select edit expression.
00:41
This displays a new dialogue which allows me to use tool or operation parameters
00:45
as well as combine these parameters with
00:47
mathematical functions such as min and max.
00:51
So let's set the step down equal to 80% of the tool flute length.
00:54
This will ensure we don't rub on the shank of the
00:56
tool against the part while still maximizing the tool's cutting potential
01:00
to help define expressions as you start typing parameters,
01:03
an autocomplete dialogue is displayed to help you find the right parameter.
01:08
Once you press OK, the numeric value of your expression is displayed
01:12
expressions capture your programming intent.
01:14
So if I change the tool in this case,
01:16
a half inch diameter flat end mill the step down
01:19
value will automatically update to 0.96 inch for this tool.
01:25
Now once you have all your parameters dialed in,
01:27
you can also set defaults for individual parameters or the entire tool path.
01:31
In this case,
01:32
if I right click on the step down and make default
01:35
all future two D contour operations will have a step down.
01:38
That is 80% of the tool flute length.
01:41
If I make all default, all parameters will be made default for this operation.
01:47
If for any reason,
01:48
you want to return to the original default reset to
01:50
built in default will return to the factory setting.
01:53
Finally, fusion 360 allows you to import and export default parameters.
01:58
So you can quickly share best practices within your shop.
02:02
Next up patterns,
02:04
patterns quickly duplicate tool paths within a single part or
02:07
across multiple parts like we have in this tombstone.
02:10
To create a pattern. We need to select the tool path.
02:12
We want to be included in the pattern, right click and select add to new pattern.
02:18
The first pattern is linear which creates a linear array
02:22
using directions selected graphically using the model sketch or geometry.
02:26
A manual spacing parameter to define separation and the number of instances.
02:32
The final parameter on the pattern tab is operation order which allows us
02:35
to specify whether we want to order the tool paths by tool which
02:39
will minimize tool changes by operation which will machine all instances of a
02:43
particular operation before moving on to the next tool path or preserve order.
02:48
So machine operations in each instance of the pattern before moving on to the next.
02:53
Now let's change the pattern type to circular and define the
02:56
rotational center for the pattern as the model origin Z axis
03:01
with an angle of 360 degrees.
03:03
In two instances,
03:04
you can see that we have successfully programmed one
03:07
of the parts on the reverse of our tombstone.
03:11
If we change the pattern type to mirror, we need to define the mirror plane,
03:15
we can use the XZ plane of this model origin.
03:17
And once again, we have programmed a component on the other side of the tombstone
03:22
note that this will also create a mirror of the original.
03:25
So this is useful for left and right parts
03:29
also note that the
03:30
towpath direction is also mirrored. So if the original tool
03:33
pa is climb cutting, the mirrored tool path will be conventional cutting
03:38
to prevent this duplicate all the tool paths you want to mirror
03:41
and add them to a mirror pattern where you uncheck keep original,
03:45
change the tool pass in that pattern to be conventional cutting
03:48
compare net it could be used to speed up this process.
03:51
Now, the pattern tool path will climb mill as desired.
03:55
A duplication pattern allows you to use geometry to pattern the selected
03:59
tool paths first select the source point from the original model.
04:03
Now, we can set the target points
04:05
as we have multiple models positioned in our tombstone.
04:07
We can select the same point on the target models.
04:10
We don't have the ability to specify any rotations with the duplication pattern.
04:14
So both the original and target model need to share the same orientation.
04:20
The last type of pattern is a component pattern which
04:22
is going to allow us to specify a source component
04:25
and it will automatically apply the specified tool paths to
04:28
all instances of the selected component in our assembly.
04:31
This time adjusting for different orientations.
04:35
If you only want to apply to certain instances,
04:38
you can deactivate automatic and manually select the target components.
04:43
The post process tab allows us to override the work coord the
04:47
system offset from what we specified in the setup if needed.
04:52
Next tool path templates help streamline the programming process by storing
04:57
a group of tool paths that you can apply later on
04:59
capturing not only your intent but a full process
05:02
to create a template.
05:03
I'll select the operations I want to include right click and stores template,
05:09
give the template a descriptive name and it
05:11
is automatically stored in your cloud template library.
05:14
If you enabled cloud libraries which we cover in the tour of the user interface.
05:18
Back at the torque plate, we can right click on the setup,
05:21
create from template and choose the template.
05:23
We just saved
05:25
tool
05:26
pas that don't rely on selections will regenerate successfully while
05:29
those that need contour selections will need to be edited.
05:33
However, all other customizations have been saved in the template.
05:37
So even if a small amount of resection is needed,
05:40
plenty of time was saved by capturing my process in the tool path template.
05:45
If I do want to make any changes to my tool path, such as changing the tool,
05:49
they are still fully customizable.
05:52
If you always find yourself using the same tool paths on every part with the
05:55
same tool path settings and options templates are
05:58
a great way to save time programming.
06:01
Now that we're ready to create some code, the final tip is NC programs.
06:05
NC programs are an alternative to the post process
06:08
option and offers several benefits including robust post selection,
06:12
clear post property settings,
06:14
grouping tool paths for multiple setups and transparent tool path ordering
06:19
in the settings.
06:19
Tab, I'll set the program name, comment and choose a local output folder.
06:24
When selecting a post,
06:26
I search for my desired post from the list of over 100 pre installed posts,
06:30
browse to a personal post.
06:31
Or I can even choose to download one from the free library of online post processors.
06:37
The properties tab displays post properties for the post I've selected.
06:41
So it keeps the page clean and easy to understand.
06:43
Post property selection are sticky even when program changes
06:46
are made or the design is opened and closed.
06:50
Lastly,
06:51
we have the operations tab which is where I can
06:53
select the tool path to include in this NC program.
06:55
For this one,
06:56
I want to output every tool path from both the bracket and torque plate setups.
07:01
When I check minimize tool changes,
07:03
the operation order changes to improve
07:05
our machining efficiency and our overall productivity
07:08
and the list updates visually to clearly show me the updated order.
07:12
The NC program appears in the browser and I could rename it for clarity
07:17
by right clicking.
07:18
I can also perform a simulation which simulates
07:20
the operation in their new optimized order.
07:24
We can also create a setup sheet which saves a PDF file directly
07:28
in the data management console and it is directly linked to our design.
07:32
Lastly,
07:33
we can choose to post process our NC program which automatically creates
07:36
a G code file in the output location with these settings.
07:39
In operation order replied,
07:41
if we make any changes to any of our operations,
07:43
there is no need to recreate the NC program, we simply need to repost the code.
07:49
So if I change the tool for the outer finishing tool path to a quarter inch,
07:53
you can see that the NC program is automatically
07:55
updated and the operation order reflects this tool change
Video transcript
00:04
Everyone wants to be more productive from the principles of lean manufacturing
00:07
to shaving seconds off machine cycle times and programming is no different.
00:11
This tutorial will cover some of the productivity tips that will
00:13
save you time when programming your parts in fusion 360.
00:17
For the first tip,
00:18
let's edit this two D contour operation that
00:21
is finishing the outer contour of this bracket
00:23
in the passes tab.
00:24
You can see that we have enabled multiple depths
00:26
to split the tool path into several step downs
00:30
while hard coding 250 that will work,
00:32
it will always be that value even if there's a change to the tool.
00:35
So instead of simply typing in a value to the step down,
00:38
I can right click and select edit expression.
00:41
This displays a new dialogue which allows me to use tool or operation parameters
00:45
as well as combine these parameters with
00:47
mathematical functions such as min and max.
00:51
So let's set the step down equal to 80% of the tool flute length.
00:54
This will ensure we don't rub on the shank of the
00:56
tool against the part while still maximizing the tool's cutting potential
01:00
to help define expressions as you start typing parameters,
01:03
an autocomplete dialogue is displayed to help you find the right parameter.
01:08
Once you press OK, the numeric value of your expression is displayed
01:12
expressions capture your programming intent.
01:14
So if I change the tool in this case,
01:16
a half inch diameter flat end mill the step down
01:19
value will automatically update to 0.96 inch for this tool.
01:25
Now once you have all your parameters dialed in,
01:27
you can also set defaults for individual parameters or the entire tool path.
01:31
In this case,
01:32
if I right click on the step down and make default
01:35
all future two D contour operations will have a step down.
01:38
That is 80% of the tool flute length.
01:41
If I make all default, all parameters will be made default for this operation.
01:47
If for any reason,
01:48
you want to return to the original default reset to
01:50
built in default will return to the factory setting.
01:53
Finally, fusion 360 allows you to import and export default parameters.
01:58
So you can quickly share best practices within your shop.
02:02
Next up patterns,
02:04
patterns quickly duplicate tool paths within a single part or
02:07
across multiple parts like we have in this tombstone.
02:10
To create a pattern. We need to select the tool path.
02:12
We want to be included in the pattern, right click and select add to new pattern.
02:18
The first pattern is linear which creates a linear array
02:22
using directions selected graphically using the model sketch or geometry.
02:26
A manual spacing parameter to define separation and the number of instances.
02:32
The final parameter on the pattern tab is operation order which allows us
02:35
to specify whether we want to order the tool paths by tool which
02:39
will minimize tool changes by operation which will machine all instances of a
02:43
particular operation before moving on to the next tool path or preserve order.
02:48
So machine operations in each instance of the pattern before moving on to the next.
02:53
Now let's change the pattern type to circular and define the
02:56
rotational center for the pattern as the model origin Z axis
03:01
with an angle of 360 degrees.
03:03
In two instances,
03:04
you can see that we have successfully programmed one
03:07
of the parts on the reverse of our tombstone.
03:11
If we change the pattern type to mirror, we need to define the mirror plane,
03:15
we can use the XZ plane of this model origin.
03:17
And once again, we have programmed a component on the other side of the tombstone
03:22
note that this will also create a mirror of the original.
03:25
So this is useful for left and right parts
03:29
also note that the
03:30
towpath direction is also mirrored. So if the original tool
03:33
pa is climb cutting, the mirrored tool path will be conventional cutting
03:38
to prevent this duplicate all the tool paths you want to mirror
03:41
and add them to a mirror pattern where you uncheck keep original,
03:45
change the tool pass in that pattern to be conventional cutting
03:48
compare net it could be used to speed up this process.
03:51
Now, the pattern tool path will climb mill as desired.
03:55
A duplication pattern allows you to use geometry to pattern the selected
03:59
tool paths first select the source point from the original model.
04:03
Now, we can set the target points
04:05
as we have multiple models positioned in our tombstone.
04:07
We can select the same point on the target models.
04:10
We don't have the ability to specify any rotations with the duplication pattern.
04:14
So both the original and target model need to share the same orientation.
04:20
The last type of pattern is a component pattern which
04:22
is going to allow us to specify a source component
04:25
and it will automatically apply the specified tool paths to
04:28
all instances of the selected component in our assembly.
04:31
This time adjusting for different orientations.
04:35
If you only want to apply to certain instances,
04:38
you can deactivate automatic and manually select the target components.
04:43
The post process tab allows us to override the work coord the
04:47
system offset from what we specified in the setup if needed.
04:52
Next tool path templates help streamline the programming process by storing
04:57
a group of tool paths that you can apply later on
04:59
capturing not only your intent but a full process
05:02
to create a template.
05:03
I'll select the operations I want to include right click and stores template,
05:09
give the template a descriptive name and it
05:11
is automatically stored in your cloud template library.
05:14
If you enabled cloud libraries which we cover in the tour of the user interface.
05:18
Back at the torque plate, we can right click on the setup,
05:21
create from template and choose the template.
05:23
We just saved
05:25
tool
05:26
pas that don't rely on selections will regenerate successfully while
05:29
those that need contour selections will need to be edited.
05:33
However, all other customizations have been saved in the template.
05:37
So even if a small amount of resection is needed,
05:40
plenty of time was saved by capturing my process in the tool path template.
05:45
If I do want to make any changes to my tool path, such as changing the tool,
05:49
they are still fully customizable.
05:52
If you always find yourself using the same tool paths on every part with the
05:55
same tool path settings and options templates are
05:58
a great way to save time programming.
06:01
Now that we're ready to create some code, the final tip is NC programs.
06:05
NC programs are an alternative to the post process
06:08
option and offers several benefits including robust post selection,
06:12
clear post property settings,
06:14
grouping tool paths for multiple setups and transparent tool path ordering
06:19
in the settings.
06:19
Tab, I'll set the program name, comment and choose a local output folder.
06:24
When selecting a post,
06:26
I search for my desired post from the list of over 100 pre installed posts,
06:30
browse to a personal post.
06:31
Or I can even choose to download one from the free library of online post processors.
06:37
The properties tab displays post properties for the post I've selected.
06:41
So it keeps the page clean and easy to understand.
06:43
Post property selection are sticky even when program changes
06:46
are made or the design is opened and closed.
06:50
Lastly,
06:51
we have the operations tab which is where I can
06:53
select the tool path to include in this NC program.
06:55
For this one,
06:56
I want to output every tool path from both the bracket and torque plate setups.
07:01
When I check minimize tool changes,
07:03
the operation order changes to improve
07:05
our machining efficiency and our overall productivity
07:08
and the list updates visually to clearly show me the updated order.
07:12
The NC program appears in the browser and I could rename it for clarity
07:17
by right clicking.
07:18
I can also perform a simulation which simulates
07:20
the operation in their new optimized order.
07:24
We can also create a setup sheet which saves a PDF file directly
07:28
in the data management console and it is directly linked to our design.
07:32
Lastly,
07:33
we can choose to post process our NC program which automatically creates
07:36
a G code file in the output location with these settings.
07:39
In operation order replied,
07:41
if we make any changes to any of our operations,
07:43
there is no need to recreate the NC program, we simply need to repost the code.
07:49
So if I change the tool for the outer finishing tool path to a quarter inch,
07:53
you can see that the NC program is automatically
07:55
updated and the operation order reflects this tool change
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.