facemill

[camtd]

Hi


When I create a facemill toolpath the default is to transition between cuts at a sharp 90 degree angle.


How can I loop the toolpath between cuts?


Thank You

 

[appinmi]

If you are trying to do something like:


View attachment 2195


You must use a trajectory sequence and either "sketch" the toolpath, or have the tool follow a datum curve.

 

[camtd]

Hi


That is exactly what I am looking do. I was hoping the facing sequence would have a toggle someplace to loop.


So the only way to get a facing toolpath like that would be in trajectory and surface machining. Does surface machining have any benifits or disadvantages?


I know very little about thetrajectory sequence. It seems that it is most used for 2d curve machining. Is that correct or is the more to it?


Thank You

 

[appinmi]

There are several ways to create a tool path in trajectory sequences:


Sketch: The tool wil follow whatever sketch you create, no matter what plane you create the sketch on. This can be useful in many places, but I use it mostly because you can "customize" your tool path more easily.You can even simulate a boring bar going straight down in "Z" changingn the feed rates as it moves down.


Curve: Just about the same as a "sketch", but the curve must be created before the sequence. I use this a lot to follow fillets in a "hog out" that don't appear on the model. (Create offset surfaces from the model & "intersect" them to create the curve). This can even be done to make the toolpath follow all 5 axis at the same time.


Edge: You can pick edges from the model that you want the cutter to follow. You can offset the tool path so it simulates a "profile" type of cut. Again, you can customize this type of cut also.


Surface: Pretty much like doing a "profile". This can come in real handy if you need to "profile" a 4 or 5 axis surface.


I did the following with "sketches". The first sketch is the lead in at the top. Added a CL command "CUTCOM/LEFT" after the "auto plunge" Then added asecond cut which is the circle at the bottom with a "helical" lead-in. I deleted the "Retract" and the "Auto Plunge" for the second cut, thus the second cut starts at the endpoint of the first cut. Then I added a "lead out", another CL command "CUTCOM/OFF",a "Go Delta", and a "Retract". This whole cut goes in and out of cutter comp only once. Yes, I know that you can create this as a "profile" with steps, but you have a lead-in and a lead-out at each step. Lead-ins and -outs cut nothing but air! When cutting high production jobs, every second saved earns money.


View attachment 2199


You can also do something similar to this, "in reverse", to cut threads with a Thread mill.

 

[marker4x4]

When I create a facemill toolpath the default is to transition between cuts at a sharp 90 degree angle. How can I loop the toolpath between cuts?

If your reason for the loop is to use high-speed machining, then yes, you have to Trajectory this.
But if you simply want to avoid the cut direction change for cosmetic / surface finish purposes, then you can specify your Facing parameters to get this:



View attachment 2210

I hope it helps,