Use the Hole Recognition strategy in conjunction with tool libraries and templates to optimize machining of holes.
Transcript
00:03
Within the Manufacturing Extension,
00:06
the Hole Recognition strategy automates the process of creating hole machining operations in both primary and multi-axis machining.
00:14
The function can evaluate multiple hole sizes to determine the best type of drilling operation to apply
00:20
and can automatically create multiple operations for each hole.
00:24
You can use templates and the tool library, along with Hole Recognition, to optimize your machining operations.
00:32
Here, you can see a component with nearly 200 holes.
00:36
As with many components, the holes are organized into various groups,
00:41
and each group is designed for different uses—for example, some holes here are tapped, some are H7 fits, and some are clearance fits.
00:51
On the Manufacture workspace toolbar, you can click Milling > Drilling > Drill to manually select the holes one by one,
00:60
choose a tool from the library, choose your settings, and then apply parameters.
01:06
However, with many holes, this process is time-consuming.
01:10
In the Drill dialog, you also have the option to Select Same Diameter holes to save some time,
01:16
but this will only find holes of the same diameter with the current tool orientation.
01:21
A more efficient process is to use the Hole Recognition strategy.
01:25
On the Manufacture workspace toolbar, click Milling > Drilling > Hole Recognition to open the Hole Recognition dialog.
01:35
While using this strategy can be as straightforward as selecting holes setting their Actions, and clicking OK,
01:41
reviewing the different options can help you to optimize this strategy.
01:46
First, identify the tools needed to create the holes for your project.
01:51
For example, to create an M6 tap hole, you need a spot drill, a 5mm drill, and an M6 tap.
01:60
On the toolbar, click Milling < Manage > Tools to open the Tool Library.
02:06
Here, you have the option to create your own tools, use personal tool libraries, import third-party libraries,
02:15
or use the Fusion sample library, which contains hundreds of free Imperial and Metric tools.
02:21
In this example, in the Tool Library, right-click Local and select Import libraries, then select the library to import from your local drive.
02:32
Once selected, click Open.
02:35
Then, in the Tool Library, click Close.
02:38
It is important to understand the role that hole signatures and templates play in Hole Recognition.
02:45
Hole signatures are the geometries that Fusion recognizes,
02:48
and include basic shapes—like cones, cylinders and flats—that make up the different types of holes.
02:56
An example of this is 2 connected cylinders, with the top larger than the bottom, connected by a flat geometry.
03:03
Together these make up a hole signature.
03:07
Hole templates are the toolpaths needed to create a specific signature.
03:11
Here, multiple tools, including a spot drill, deep drill, and a 2D bore are needed in sequence to complete this geometry,
03:20
and these toolpaths can be combined as a hole template.
03:23
For the more conventional hole signatures in a part, such as a blind tapped hole, you can use a predefined template in the Fusion library.
03:32
From the toolbar, click Milling > Manage > Templates.
03:37
In the Template Library dialog, expand Fusion Library,
03:41
and then select Holes to view the predefined templates—here, Spotdrill, Drill, & Tap Hole is selected.
03:49
Right-click the template and select Copy to copy and paste this template into your own cloud or local library.
03:56
Here, you can see one in the cloud named Custom Hole Recognition.
04:01
You can also create your own template.
04:04
Close the template Library.
04:07
In the Browser, locate the toolpaths required for your template—here, Carbide drill, Spotdrill, and Tap.
04:16
To activate the toolpaths as a hole template, select them, then right-click and select Store as Hole Template.
04:24
In the Store as template dialog, type an appropriate name for the template—here, Carbide, drill Spot to chamfer, then tap.
04:33
Add relevant details to the Description, then click Save.
04:38
To access other Milling toolpaths available for use in Hole Recognition, on the Milling tab, expand the 2D menu.
04:46
Here, you can select Thread, Bore, and Circular.
04:51
Notice that in this instance, Circular was used twice for the large holes in the part.
04:57
To use the drilling cycles, click Milling > Drilling > Drill.
05:02
On the Passes tab of the Drill dialog, expand Cycle Type and make a selection.
05:09
With the creation of any necessary templates complete, open the Hole Recognition dialog again.
05:16
Click the Tool Libraries tab to view the selected tool libraries and to set the defaults.
05:22
Open the Options tab to view or select a Template library folder.
05:27
Back on the Hole Groups tab, select a hole in the list to see the corresponding holes highlighted on the canvas,
05:34
as well as a preview of the hole signature in the dialog.
05:39
Select the appropriate Action for each hole signature.
05:44
Here, you can see holes that are automatically ignored because of their large size, or excluded based on the cut direction.
05:52
For threaded holes, select the Thread Type, if needed.
05:56
With your selections complete, click OK.
06:01
On the canvas, notice the appropriate drilling toolpaths and templates are applied in the primary axes.
06:08
You can also use Hole Recognition for multi-axis machines.
06:13
Open the Hole Recognition dialog again, and on the Options tab, select Multi-Axis Machining.
06:20
Now, you can filter based on the angle of the hole from the primary axis.
06:25
In this example, select Find by Angle, and set the Maximum Angle to 90 degrees.
06:32
On the Hole Groups tab, several extra hole groups are now added to the list.
06:37
To clean up the table view, select Hide ignored groups.
06:42
Return to the Options tab, where you can filter based on size, limit the Thread Size Tolerance, Include Partial Holes,
06:50
Organize Operations based on either Minimizing tool changes or Grouping by size, and Use Fewest Spot Drills Possible.
06:60
Back on the Hole Groups tab, you can also explode hole groups.
07:04
This is useful if you have signatures that are the same in your CAD model, but different in reality.
07:10
For example, looking at these central holes, the 2 outer holes may be blind tapped holes, while the middle one may be a reamed hole.
07:18
Select the hole group, then click Explode Select Hole Groups.
07:22
Now, in the list, select the holes you want to be tapped, then right-click and select the appropriate hole template.
07:33
Do the same for the remaining holes.
07:38
You also have the option to Delete Top Segment, Delete Bottom Segment, Split Hole Signature, or Flip Hole direction.
07:47
When all setup is complete, click OK.
07:51
Now you understand how to use Hole Recognition in conjunction with tool libraries and hole templates
07:57
to automate drilling of holes in both primary and multi-axis machining.
00:03
Within the Manufacturing Extension,
00:06
the Hole Recognition strategy automates the process of creating hole machining operations in both primary and multi-axis machining.
00:14
The function can evaluate multiple hole sizes to determine the best type of drilling operation to apply
00:20
and can automatically create multiple operations for each hole.
00:24
You can use templates and the tool library, along with Hole Recognition, to optimize your machining operations.
00:32
Here, you can see a component with nearly 200 holes.
00:36
As with many components, the holes are organized into various groups,
00:41
and each group is designed for different uses—for example, some holes here are tapped, some are H7 fits, and some are clearance fits.
00:51
On the Manufacture workspace toolbar, you can click Milling > Drilling > Drill to manually select the holes one by one,
00:60
choose a tool from the library, choose your settings, and then apply parameters.
01:06
However, with many holes, this process is time-consuming.
01:10
In the Drill dialog, you also have the option to Select Same Diameter holes to save some time,
01:16
but this will only find holes of the same diameter with the current tool orientation.
01:21
A more efficient process is to use the Hole Recognition strategy.
01:25
On the Manufacture workspace toolbar, click Milling > Drilling > Hole Recognition to open the Hole Recognition dialog.
01:35
While using this strategy can be as straightforward as selecting holes setting their Actions, and clicking OK,
01:41
reviewing the different options can help you to optimize this strategy.
01:46
First, identify the tools needed to create the holes for your project.
01:51
For example, to create an M6 tap hole, you need a spot drill, a 5mm drill, and an M6 tap.
01:60
On the toolbar, click Milling < Manage > Tools to open the Tool Library.
02:06
Here, you have the option to create your own tools, use personal tool libraries, import third-party libraries,
02:15
or use the Fusion sample library, which contains hundreds of free Imperial and Metric tools.
02:21
In this example, in the Tool Library, right-click Local and select Import libraries, then select the library to import from your local drive.
02:32
Once selected, click Open.
02:35
Then, in the Tool Library, click Close.
02:38
It is important to understand the role that hole signatures and templates play in Hole Recognition.
02:45
Hole signatures are the geometries that Fusion recognizes,
02:48
and include basic shapes—like cones, cylinders and flats—that make up the different types of holes.
02:56
An example of this is 2 connected cylinders, with the top larger than the bottom, connected by a flat geometry.
03:03
Together these make up a hole signature.
03:07
Hole templates are the toolpaths needed to create a specific signature.
03:11
Here, multiple tools, including a spot drill, deep drill, and a 2D bore are needed in sequence to complete this geometry,
03:20
and these toolpaths can be combined as a hole template.
03:23
For the more conventional hole signatures in a part, such as a blind tapped hole, you can use a predefined template in the Fusion library.
03:32
From the toolbar, click Milling > Manage > Templates.
03:37
In the Template Library dialog, expand Fusion Library,
03:41
and then select Holes to view the predefined templates—here, Spotdrill, Drill, & Tap Hole is selected.
03:49
Right-click the template and select Copy to copy and paste this template into your own cloud or local library.
03:56
Here, you can see one in the cloud named Custom Hole Recognition.
04:01
You can also create your own template.
04:04
Close the template Library.
04:07
In the Browser, locate the toolpaths required for your template—here, Carbide drill, Spotdrill, and Tap.
04:16
To activate the toolpaths as a hole template, select them, then right-click and select Store as Hole Template.
04:24
In the Store as template dialog, type an appropriate name for the template—here, Carbide, drill Spot to chamfer, then tap.
04:33
Add relevant details to the Description, then click Save.
04:38
To access other Milling toolpaths available for use in Hole Recognition, on the Milling tab, expand the 2D menu.
04:46
Here, you can select Thread, Bore, and Circular.
04:51
Notice that in this instance, Circular was used twice for the large holes in the part.
04:57
To use the drilling cycles, click Milling > Drilling > Drill.
05:02
On the Passes tab of the Drill dialog, expand Cycle Type and make a selection.
05:09
With the creation of any necessary templates complete, open the Hole Recognition dialog again.
05:16
Click the Tool Libraries tab to view the selected tool libraries and to set the defaults.
05:22
Open the Options tab to view or select a Template library folder.
05:27
Back on the Hole Groups tab, select a hole in the list to see the corresponding holes highlighted on the canvas,
05:34
as well as a preview of the hole signature in the dialog.
05:39
Select the appropriate Action for each hole signature.
05:44
Here, you can see holes that are automatically ignored because of their large size, or excluded based on the cut direction.
05:52
For threaded holes, select the Thread Type, if needed.
05:56
With your selections complete, click OK.
06:01
On the canvas, notice the appropriate drilling toolpaths and templates are applied in the primary axes.
06:08
You can also use Hole Recognition for multi-axis machines.
06:13
Open the Hole Recognition dialog again, and on the Options tab, select Multi-Axis Machining.
06:20
Now, you can filter based on the angle of the hole from the primary axis.
06:25
In this example, select Find by Angle, and set the Maximum Angle to 90 degrees.
06:32
On the Hole Groups tab, several extra hole groups are now added to the list.
06:37
To clean up the table view, select Hide ignored groups.
06:42
Return to the Options tab, where you can filter based on size, limit the Thread Size Tolerance, Include Partial Holes,
06:50
Organize Operations based on either Minimizing tool changes or Grouping by size, and Use Fewest Spot Drills Possible.
06:60
Back on the Hole Groups tab, you can also explode hole groups.
07:04
This is useful if you have signatures that are the same in your CAD model, but different in reality.
07:10
For example, looking at these central holes, the 2 outer holes may be blind tapped holes, while the middle one may be a reamed hole.
07:18
Select the hole group, then click Explode Select Hole Groups.
07:22
Now, in the list, select the holes you want to be tapped, then right-click and select the appropriate hole template.
07:33
Do the same for the remaining holes.
07:38
You also have the option to Delete Top Segment, Delete Bottom Segment, Split Hole Signature, or Flip Hole direction.
07:47
When all setup is complete, click OK.
07:51
Now you understand how to use Hole Recognition in conjunction with tool libraries and hole templates
07:57
to automate drilling of holes in both primary and multi-axis machining.
