An overview of the basic milling toolpath parameters using the Face milling strategy.
Transcript
00:07
It is sometimes called 2.5-axis machining
00:11
because all the cuts are limited to a 2-axis plane—normally the XY plane—and then the depth cuts are taken in the third axis,
00:19
normally the Z axis.
00:22
In the Manufacture workspace, Milling toolbar,
00:26
expand the 2D menu to see the variety of toolpaths available to represent this type of machining.
00:32
This example will focus on the Face toolpath.
00:36
Face, or facing, is the process of milling the rough stock off the top of the part to make it flat.
00:44
Select Face to open the Face dialog, which is divided into five tabs:
00:49
The Tool tab is where you can select the cutting tool and type of coolant, and define the cutting feeds and speeds.
00:57
On the Geometry tab, you can select the boundary or area to be machined, the stock area, and any areas to exclude from machining.
01:07
These options change depending on the toolpath selected, but generally, the Geometry tab is used to select the cutting area.
01:16
The Heights tab is where you can set all the Z-position heights for the rapid clearance, the top of the part, the retract position,
01:25
and the bottom of the cut or final depth.
01:28
The Passes tab contains cutting parameters, the width of the cut, multiple depth cuts, stock to leave,
01:36
and toolpath smoothing, which is used to filter linear moves into arc moves, where possible.
01:42
These parameters also vary depending on the selected toolpath.
01:48
The Linking tab controls how the tool positions when the cutter must retract from a cut and position for the next cut.
01:56
These parameters also control how the tool will blend onto the cut and off using the leads and transitions.
02:04
Again, there will be some minor variations in these parameters, depending on which toolpath strategy is selected.
02:12
In most cases, the Fusion system defaults produce an excellent toolpath, requiring few changes.
02:20
Switch back to the Tool tab to define the facing cuts for this example part.
02:25
In the Tool group, click Select to open the Tool Library.
02:30
The Tool Library dialog is divided into three general sections:
02:35
The available libraries on the left, Tool filters and information on the right, and the available tools in the middle.
02:44
Within the available libraries section, under Documents, you see the currently open documents.
02:51
Fusion Library shows the tool libraries included with Fusion.
02:56
Under Local and Cloud, you see any custom libraries created by you or your Team Hub members, respectively.
03:04
This sample part has tools already created.
03:08
Expand the Document heading and select Intro to 2D Machining to show the tools for this document.
03:15
Select tool 1 (2” Face Mill) from the list, and then click Select.
03:22
In the Face dialog, Tool tab, leave the default Feed & Speed settings, and switch to the Geometry tab.
03:31
This is where you select the profile to be machined.
03:35
For Face milling, you generally want to clean off the entire top of the stock.
03:40
Fusion assumes this and shows the stock boundary.
03:45
Place your pointer over group headings or individual parameters to see detailed tooltips with useful text and illustrations.
03:54
For the Stock Contours group heading,
03:56
the tooltip explains that there is nothing for you to pick unless you want to select a specific area to face.
04:03
Place your pointer over the Stock Selections box, and the tooltip explains what you can select and how the toolpath results may look.
04:12
Leave these Geometry settings set to the defaults.
04:16
Switch to the Heights tab.
04:19
From here, you can set clearance positions and depths in the spindle axis, normally the Z-axis:
04:26
The Clearance Height is the fully retracted position above the part.
04:30
It represents the safest height the tool can position.
04:34
This is the Z-height for the first rapid position and the last height after the toolpath has been completed.
04:41
The Retract Height is the intermediate position where the tool retracts between cuts, when taking multiple cuts on a profile or pocket.
04:51
The Feed Height is where the tool starts its feed move to the cutting depth or the start of the pecks, for multiple depth cuts.
04:59
Normally, this is the minimum distance above the material to be removed.
05:04
The Top Height defines the actual top of the surface to be machined.
05:09
It is the top of the material to be removed.
05:13
The Bottom Height is the final cut depth.
05:17
Each of these heights can have a different reference.
05:21
Some positions will be in reference to the model, and some will be in reference to the stock you defined in the setup.
05:29
Some heights can be in reference to other heights, so when you specify the Offset value for the heights,
05:35
you could also set the From reference.
05:38
Place your pointer over the From inputs, to view a tooltip with reference options.
05:44
It is best not to think of these as an absolute Z-position, but rather as a reference to the model.
05:51
This is the benefit of an associative toolpath.
05:55
If the model changes, the heights can maintain their reference.
05:60
You can also adjust the height offset values directly in the model by dragging the colored rectangles up or down.
06:07
Move the Retract Height rectangle, and notice that the Clearance Height moves as well.
06:13
This is because the Clearance Height is in reference to the Retract Height.
06:18
For this example, you do not need to adjust any height parameters.
06:23
The Top Height is in reference to the Stock top and the Bottom Height is in reference to the Model top.
06:31
This means that the amount of stock on the top of the part is the amount it will be facing off.
06:37
Switch to the Passes tab to control the cutting steps.
06:41
For facing, you can control the Pass Direction for the first cut, the Pass Extension off the edge, and the Stepover between cuts.
06:51
You can also select between cutting in both directions or only one way.
06:57
For this example, set the Pass Extension to 1 inch, which is half the cutter diameter,
07:03
and the Stepover to 1.8, almost the full width of the cutter.
07:07
The block is only 1.75 inches wide, so these settings should enable a single cut across the top face.
07:16
Switch to the Linking tab to control motion between multiple cuts.
07:21
If the toolpath is generating many small cuts, that may create many retract moves.
07:27
You can limit the number of retracts and how it transitions between the cuts using these parameters.
07:34
If the area has many ribs or pockets, you may need a full retract to the clearance height.
07:41
If the area is generally open, there may be no need for a full retract.
07:46
By evaluating the distance from the end of one cut to the start of the next, Fusion can determine if a full retract should be output.
07:56
By increasing the Maximum Stay-Down Distance,
07:59
you can reduce the number of retracts and instead replace them with feed moves to the start of the next cut.
08:06
In the tooltip, you see that increasing the Maximum Stay-Down Distance keeps the tool closer down in the cavity.
08:13
Staying closer to the cavity will most likely reduce the cycle time as well.
08:19
The Linking tab also contains Leads & Transitions settings.
08:24
This sets how it will lead onto the first cut or lead off the last cut.
08:29
Set the Vertical Lead-In Radius value to 0.2, which is preferred for leading into a very tight area.
08:38
Click OK to generate the toolpath.
08:41
Save your model if you want to continue working on it.
00:07
It is sometimes called 2.5-axis machining
00:11
because all the cuts are limited to a 2-axis plane—normally the XY plane—and then the depth cuts are taken in the third axis,
00:19
normally the Z axis.
00:22
In the Manufacture workspace, Milling toolbar,
00:26
expand the 2D menu to see the variety of toolpaths available to represent this type of machining.
00:32
This example will focus on the Face toolpath.
00:36
Face, or facing, is the process of milling the rough stock off the top of the part to make it flat.
00:44
Select Face to open the Face dialog, which is divided into five tabs:
00:49
The Tool tab is where you can select the cutting tool and type of coolant, and define the cutting feeds and speeds.
00:57
On the Geometry tab, you can select the boundary or area to be machined, the stock area, and any areas to exclude from machining.
01:07
These options change depending on the toolpath selected, but generally, the Geometry tab is used to select the cutting area.
01:16
The Heights tab is where you can set all the Z-position heights for the rapid clearance, the top of the part, the retract position,
01:25
and the bottom of the cut or final depth.
01:28
The Passes tab contains cutting parameters, the width of the cut, multiple depth cuts, stock to leave,
01:36
and toolpath smoothing, which is used to filter linear moves into arc moves, where possible.
01:42
These parameters also vary depending on the selected toolpath.
01:48
The Linking tab controls how the tool positions when the cutter must retract from a cut and position for the next cut.
01:56
These parameters also control how the tool will blend onto the cut and off using the leads and transitions.
02:04
Again, there will be some minor variations in these parameters, depending on which toolpath strategy is selected.
02:12
In most cases, the Fusion system defaults produce an excellent toolpath, requiring few changes.
02:20
Switch back to the Tool tab to define the facing cuts for this example part.
02:25
In the Tool group, click Select to open the Tool Library.
02:30
The Tool Library dialog is divided into three general sections:
02:35
The available libraries on the left, Tool filters and information on the right, and the available tools in the middle.
02:44
Within the available libraries section, under Documents, you see the currently open documents.
02:51
Fusion Library shows the tool libraries included with Fusion.
02:56
Under Local and Cloud, you see any custom libraries created by you or your Team Hub members, respectively.
03:04
This sample part has tools already created.
03:08
Expand the Document heading and select Intro to 2D Machining to show the tools for this document.
03:15
Select tool 1 (2” Face Mill) from the list, and then click Select.
03:22
In the Face dialog, Tool tab, leave the default Feed & Speed settings, and switch to the Geometry tab.
03:31
This is where you select the profile to be machined.
03:35
For Face milling, you generally want to clean off the entire top of the stock.
03:40
Fusion assumes this and shows the stock boundary.
03:45
Place your pointer over group headings or individual parameters to see detailed tooltips with useful text and illustrations.
03:54
For the Stock Contours group heading,
03:56
the tooltip explains that there is nothing for you to pick unless you want to select a specific area to face.
04:03
Place your pointer over the Stock Selections box, and the tooltip explains what you can select and how the toolpath results may look.
04:12
Leave these Geometry settings set to the defaults.
04:16
Switch to the Heights tab.
04:19
From here, you can set clearance positions and depths in the spindle axis, normally the Z-axis:
04:26
The Clearance Height is the fully retracted position above the part.
04:30
It represents the safest height the tool can position.
04:34
This is the Z-height for the first rapid position and the last height after the toolpath has been completed.
04:41
The Retract Height is the intermediate position where the tool retracts between cuts, when taking multiple cuts on a profile or pocket.
04:51
The Feed Height is where the tool starts its feed move to the cutting depth or the start of the pecks, for multiple depth cuts.
04:59
Normally, this is the minimum distance above the material to be removed.
05:04
The Top Height defines the actual top of the surface to be machined.
05:09
It is the top of the material to be removed.
05:13
The Bottom Height is the final cut depth.
05:17
Each of these heights can have a different reference.
05:21
Some positions will be in reference to the model, and some will be in reference to the stock you defined in the setup.
05:29
Some heights can be in reference to other heights, so when you specify the Offset value for the heights,
05:35
you could also set the From reference.
05:38
Place your pointer over the From inputs, to view a tooltip with reference options.
05:44
It is best not to think of these as an absolute Z-position, but rather as a reference to the model.
05:51
This is the benefit of an associative toolpath.
05:55
If the model changes, the heights can maintain their reference.
05:60
You can also adjust the height offset values directly in the model by dragging the colored rectangles up or down.
06:07
Move the Retract Height rectangle, and notice that the Clearance Height moves as well.
06:13
This is because the Clearance Height is in reference to the Retract Height.
06:18
For this example, you do not need to adjust any height parameters.
06:23
The Top Height is in reference to the Stock top and the Bottom Height is in reference to the Model top.
06:31
This means that the amount of stock on the top of the part is the amount it will be facing off.
06:37
Switch to the Passes tab to control the cutting steps.
06:41
For facing, you can control the Pass Direction for the first cut, the Pass Extension off the edge, and the Stepover between cuts.
06:51
You can also select between cutting in both directions or only one way.
06:57
For this example, set the Pass Extension to 1 inch, which is half the cutter diameter,
07:03
and the Stepover to 1.8, almost the full width of the cutter.
07:07
The block is only 1.75 inches wide, so these settings should enable a single cut across the top face.
07:16
Switch to the Linking tab to control motion between multiple cuts.
07:21
If the toolpath is generating many small cuts, that may create many retract moves.
07:27
You can limit the number of retracts and how it transitions between the cuts using these parameters.
07:34
If the area has many ribs or pockets, you may need a full retract to the clearance height.
07:41
If the area is generally open, there may be no need for a full retract.
07:46
By evaluating the distance from the end of one cut to the start of the next, Fusion can determine if a full retract should be output.
07:56
By increasing the Maximum Stay-Down Distance,
07:59
you can reduce the number of retracts and instead replace them with feed moves to the start of the next cut.
08:06
In the tooltip, you see that increasing the Maximum Stay-Down Distance keeps the tool closer down in the cavity.
08:13
Staying closer to the cavity will most likely reduce the cycle time as well.
08:19
The Linking tab also contains Leads & Transitions settings.
08:24
This sets how it will lead onto the first cut or lead off the last cut.
08:29
Set the Vertical Lead-In Radius value to 0.2, which is preferred for leading into a very tight area.
08:38
Click OK to generate the toolpath.
08:41
Save your model if you want to continue working on it.
Manufacture > Milling > 2D > 2D Face 
2D Face Milling is planer machining process. It's sometimes called 2.5 axis machining because all of the cuts are limited to a 2 axis plane (normally XY) and the depth cuts are taken in the 3rd axis (normally Z). When you select the 2D pull down, there are a variety of toolpaths that represent this type of machining.
Toolpath Parameters This video is includes an overview of the toolpath dialogs. It discusses their similarities and differences.
