Machining corners in graphite electrodes

[Anonymous]

Would anyone here want to give advice or share a PowerMill project they use for machining graphite electrodes?  We are having trouble with sharp inside corners.  We tend to get small gouges.  We make thousands of these a year with every one of them different.  I have a macro that I've set up to calculate them automatically, and then afterwards we open it up to review and tweak them as needed.

I do not currently use one of the corner finishing strategies because it doesn't seem reliable.  For example, I have a 1/16 ball that is rest finishing what the previous tool (1/8 ball) cannot get.  My toolpath looks like so.  Note the circled area.

.

If I try an automatic corner finishing toolpath, I get this.  Leads and links turned off for clarity.

.

Note how it doesn't attempt to get that area at all.

Is it better to use a combination of toolpaths to get the corners?  I don't really think the corner finishing would improve the gouging much anyway.  I have thought about using a constant Z inside the boundary and using the high speed option, but then how do you reference that for the next smaller tool?

Any help would be appreciated.

[iamcdn79]

Normally what I would use on graphite is to use optimized constant z over the entire model using the smallest tool needed (Diamond coated) that would finish all the smaller corners. That stratagey works 90% of the time for me.

Another stratagey that I would use if optimized constant z doesn't work is steep/shallow over the entire model with the smallest cutter. The only problem with steep/shallow is the 3d offset portion for shallow areas starts from the inside out. Would need to select those areas manually  with a macro provided from @5axes found here if you want to start from the outside and work your way in

Finishing the entire model with the smallest tools eliminates blending issues and corner picking.

The only downfall with that is it can take alot of machining time if its a large model, and hopefully you don't need long tools for deep models

[Anonymous]

Occasionally we do cut it all with the smallest cutter, but that's not reasonable most of the time because of how long it takes.  We use cutters as small as .015" quite commonly, and they run fairly slow.

[iamcdn79]

Smallest cutter we go down to is 1 mm and that is rarely, usually, 1/16 or 1/8 is good enough

Try steep/shallow or optimized constant z in your project snapshot provided

[kandennti]

HI jacob.seppanen.

This problem can be found in other CAM software as well.
Please search by "inverse offset method".
I do not know but I think it is a problem with this algorithm.

[Anonymous]

The first screenshot in my initial post is a steep/shallow toolpath, which is what I currently use.  Optimized Z gives similar results.  Ideally there would be a high speed arc fit corners option within one of those toolpaths, but I think that has been on the wishlist for many years already.  I'm guessing it must not be an easy thing to do.

[iamcdn79]

Can you upload the project?

[Anonymous]

Hmm... It fails when I try to upload it and post.  I think it must be the file size.  22MB  Any idea what the limit is for uploads here?  I will try to make a simplified version of it.

[iamcdn79]

Are you zipping the project?

[Anonymous]

I'm saving as an archived project which is essentially the same as zipping it I think but in a PowerMill format.  I'll try zipping it to see if it's any smaller.

[Anonymous]

I can't seem to get the file size small enough.  I had it under 10MB and it still rejected it.  Try this:  https://spaces.hightail.com/receive/Z3XpPNLCJV   Once downloaded, click file>open>archived project from within PowerMill.

[iamcdn79]

I looked at your project and can't see what the issue would be in your provided snapshot. The toolpath looks good to me. Is your issue with it that you can't add arcs to the corners? 

I've noticed that you have your links set to incremental, is there a reason you're using that and not skim?

I would also suggest adding circular arcs to your first skim choice instead of skim to keep the tool down see attached pic of before and after

[Anonymous]

I will look into the leads/links things you suggest.  The real issue is that the vertical corners tend to have small gouges in the transitions from one tool size to the next.  If some sort of arc-fitting were possible in the corners, I think that would eliminate the problem.  Since it really isn't other than constant Z (which would open up other problems) I am hoping to find a better way to program the corners to avoid that somehow.  The screenshots were an example of what I currently use, how I tried to use one of the corner finishing strategies as someone at Autodesk had suggested to me, and why that fails in my opinion.

[iamcdn79]

Ya unfortunately arc fit corners hasn't been implemented yet to all finishing toolpaths.

There is another corner clearing strategy called corner clearance that does have the ability to add arc fit corners. I have tried it on your part but the results are not that great though.  Maybe if you tried playing around with the settings you might get better results.

[werner.do-rite]

I have been machining electrodes for 20 years using powermill.I generally use corner finishing.

When i run into problems with bad toolpath such as yours.I first create a rest boundary.Than i run a constant z

toolpath with arc fit on so i swing a radius in the corner.Than i create a shallow boundary inside the rest boundary.

I trim out the constant z toolpath to the shallow boundry to get rid of any large stepovers.Than a 3d offset toolpath with the shallow boundary.A pain in the ass doing this, but it creates good toolpath with an excellent finish.Adjust your leads and links to what the one guy said.

[iamcdn79]

When you create the 3d offset toolpath will it not gouge into the corners from the constant-z toolpath if arc-fit corners are turned on?

[werner.do-rite]

I have never had an issue with this.I usually swing a .002 arc fit radius in the corner with constant z.The constant z toolpath takes out most of the material.Then i go outside in on my 3d toolpath.I generally finish my electrode with a 4mm ball cutter.Than corner finish with a 3 mm to a 2mm to 1mm.The smallest cutter i go down to is .4mm.

[iamcdn79]

---

@werner.do-rite wrote:
I have never had an issue with this.I usually swing a .002 arc fit radius in the corner with constant z.

---

That's 2 tenths of 1% of the diameter of the tool, which is pretty small, I was thinking you were going bigger than that say like .02 and bigger

[Anonymous]

I'll definitely have to take a look at the corner clearance toolpath.  Funny how it's probably been there for years but I've never paid any attention to it.

I've considered using a constant Z with high speed, then use the next smaller tool with the constant Z, then go back with a 3D offset or order to avoid the problem in the corners as was mentioned.  Seems like a lot of toolpaths and might get messy, though.

@werner.do-rite What settings do you use for corner clearance?  Can you send me a few screenshots of your settings pages?  Or upload a copy of your strategy?

[Anonymous]

I just saw this post and thought I would point out a setting that may help.

Fist screen shot has remove deep cuts checked. The second one has it unchecked. Not sure what the software cutoff is for deep cuts but, I just double check my stock model to see if it looks ok to cut. I never had a machining issue when I have it unchecked. Hope it gives you another option for your corners.