Friday, June 19, 2015

Workaround for Plunge milling (until we get the toolpath)

What I want to show can be used the same way in Inventor, Fusion 360, and SolidWorks.
So, what i want to look at is a way to create a plunge milling toolpath without actually having the toolpath available in the software.  There are a couple of different ways that you can go about doing this.  The first option is creating a one line sketch where that line is a certain distance above the part and then goes down to a given depth inside the pocket that you are trying to plunge mill.
On your CAM ribbon under the 2D milling toolpaths select the toolpath called "Trace".  Once you have selected the tool that you want to use; go to the geometry tab and select the one line that we created in the sketch.
Once this is done, you can then create a linear pattern of the toolpath and the spacing distance would be the tool vendors recommendation on stepovers, and then the quantity would be whatever it takes to get to the end of your part.  For the part i am working with here are the values that i am using; the distance spacing is .125 in, and then the quantity is 193.
The one downfall to doing the linear patter is that it basically creates 193 operations; so, when you go to post it the output will literally show 193 operations in the code.

A second way of doing this is by creating a sketch along the length of the part and doing a one line sketch then doing a linear pattern of that one line the 193 instances.  Then create a Trace toolpath and in the geometry tab for the geometry selection go back to the model browser and select the sketch that you created.  this will automatically define all the lines in the sketch as the geometry that it needs to follow.  Then you can post out this one operation and it will make all the passes for the plunge milling.

Another option, if you are worried about chip breaking at all is to do the one line sketch and create a drill operation with the plunge milling tool.  And when in the drill operation on the geometry tab, change the selection from surfaces to "Selected Points".  With this change you can select the top point of the line and then the bottom point to actually define the depth of the toolpath.  Then move over to the "Cycle" tab and change to the cycle type that you want for Chip Breaking.  Once created you can go ahead and do the linear pattern operation.  Doing this by the drilling method doubles the cycle time compared to the Trace operation, but it is all in how you want the plunge milling to actually function.

**Disclaimer - be sure to use the vendor specified stepovers for any plunge mills!***

Good luck and Happy Programming!

No comments:

Post a Comment