Deburr Toolpath Issues

[Jake L]

Recently I have started regularly using the multiaxis deburr toolpath on many of my parts. Most of my parts are run on some form of a 3 axis vertical machine. As shown in the screenshot, when the toolpath gets to a complex edge it seems to have a hard time figuring out a smooth path. It ends up producing a very jagged toolpath which takes a lot of extra time for the machine to run. I tried playing with the surface quality tolerance, and the chaining tolerance but that only seems to help a little. I can never seem to eliminate all of the roughness. My question is, is there a way to smooth out those corners? Or is it just a matter of being a complex edge and the software can only do so much with it?

I have attached a mastercam file as an example. Please ignore speeds and feeds and other technicalities as I'm just trying to display the toolpath issues. I am running Mastercam 2022 and the tool I'm looking to use is a 1/4 diameter lollipop tool.

If more information is needed please let me know, and thanks in advance for any help anyone can give on this topic.

Deburr_Toolpath.mcam

[Chally72]

Hey Jake, thanks for uploading the file. This "noise" issue is something we spent some time addressing for 2023 to improve results. This is happening specifically in the area where those two sharp edges come together to the single edge- What happens when the lollipop transitions through that "Y" is that at some point, we need to shuffle the tool to the side so as to not violate/gouge our part beyond our allowed edge break and tolerance. 

2023 handles this a lot better and gets rid of the funky oscillation. It actually helps to loosen the tolerance back up again, so as to allow more wiggle room for the tool to overcut/gouge as it reaches those intersecting surfaces. I brought it up to 0.002" on your path and regenerated. The remaining zig you see below is the minimum necessary move to avoid chewing up the adjacent edge as we pass through the Y intersection:

And here's what it looks like for tool engagement in backplot:

 

 

[Jespertech]

In a case like this where there are blending issues I'll try to use a smaller tool to reduce the effect that Dylan pointed out above. It doesn't completely solve the issue but it does make enough of a difference to improve the toolpaths overall finish.  I changed your tool from a 1/4" to a 3/16" lollipop and I think it made a noticeable difference on that particular corner. I know that may not be an option depending on what tools you have in stock but if so its worth a shot.  

Deburr_Toolpath .187 lollipop.mcam

[Jake L]

3 minutes ago, Jespertech said:

In a case like this where there are blending issues I'll try to use a smaller tool to reduce the effect that Dylan pointed out above. It doesn't completely solve the issue but it does make enough of a difference to improve the toolpaths overall finish.

I know that may not be an option depending on what tools you have in stock but if so its worth a shot.  

That's definitely an option I'll keep in mind. It won't work for the particular project I'm on, but I'm sure I will run into this issue again. Thank you.

[Jake L]

I now have a follow up question. On the same toolpath, with the same file, the purple transition moves are broken into line segments. Is there a way to have Mastercam automatically make those arc moves? I would rather a large arc move that travels a little farther, than segments. Some of the machines read the segments slow so they can only travel so fast on those moves. I would rather an arc so the machine just has one move and can go as fast as it can go. Usually I would look for that in the toolpath in the Arc Filter / Tolerance tab but the deburr toolpath does not contain that tab.

I understand I could have the machine retract and rapid each time I have to change positions, but that is also slow because then I have to rapid out of the part every time. 

[Chally72]

Hey Jake,

Even though we're locking this to 3 axis, Deburr is still a multiaxis path in the background, whose output is restricted to linear segments- so there's no way to have this path type output arcs.

Depending on your machine, you should try going after smoothing/tolerance parameters at the control to loosen them up and allow the machine to flow through these linear segments more naturally- IE, Haas G187, Heidenhain Cycle 32, etc. Using a looser toolpath tolerance to avoid dense clumps of points will also help. That 0.0005" tolerance on your example path inserts some pretty clustered groupings that would wreak havoc on machines with no/limited smoothing and lookahead.

[Aaron Eberhard]

Another note on the Clearance Blend Spline links, for 2022 they use the Retract rates.  In 2023, you will have independent control of it:

[Jake L]

1 minute ago, Aaron Eberhard said:

Another note on the Clearance Blend Spline links, for 2022 they use the Retract rates.  In 2023, you will have independent control of it

That's awesome to hear. It took me a few minutes to figure that out when I started using this toolpath. 

What about the "Home / Ref. Points" tab? Instead of just having a clearance plane (or clearance area) will we also get an option to send the machine to a specified retract or home position after it finishes the toolpath? Or is this option already available and I just don't know it? We use reference points all the time if we want to have a retract height, a clearance height, and a large clearance height. (The large clearance height is usually used anytime we need to rotate the part in the 4th or 5th axis once the toolpath is finished). 

The only three work arounds I can currently see to this problem are to put a point toolpath in to retract the tool. Have a toolpath as shown in the picture which seems like a waste of time, especially on a larger part. Or, use the clearance blend spline, which is usually but not always the ideal method.