Serious Core Roughing Problem?

[Bruce Kanzelmeyer]

The last 2 parts I have run I have experienced a problem with the Surface High Speed, Core Roughing operation. In Linking Parameters I have always used Minimum Vertical Retract, with no issues for many years. But the last 2 parts I have run, the roughing tool has rapid moved right through the part and not cleared the part by the default 0.153". Has anyone else noticed a difference in the way Mastercam is interpreting this operation? I noticed that the default has the Output feed move box checked and I have in the past always unchecked it to create rapid moves during these linking moves. But in the last 2 parts I have run, occasionally the rapid Z retract does not move a position that clears the part. These faulty rapid moves are not picked up in Mastercam Verify, which is making me wonder if the post is interpreting these retracts differently. I can solve the issue when I run a Full Vertical Retract, but this adds a lot of extra z travel. Has anyone else seen this problem? Any suggestions for a solution? I must be overlooking something simple. Thanks for your help.

[neurosis]

Ive run in to this problem on our new Mori but it was not Mastercams fault. The Mori dog legs when it rapids so you will not see the crash during verify. Im not sure if this is the issue that you are having?

 

I fixed it by keeping the output feed move checked and using a very high feed rate.

[neurosis]

I should also add, that I have seen this problem using bullnose endmills as well but only when using optirough.

[peon]

+1 to Neuro. ALWAYS ALWAYS ALWAYS!!! keep the "Output feed move" checked when using minimum vertical retract.

[Oscar R.]

Same here. I've had a few clearence moves rapid through my part when using this toolpath. Same conditions.

Always have "output feed move" checked when using OptiRough toolpaths.

[peon]

I have seen the tool rapid through the part with Optirough and Hybrid, but never with HST Core Rough if you feed the tool. I believe Bruce was only describing the issue with HST Core Rough.

[Bruce Kanzelmeyer]

I am using a bullnose EM with .12" radius, a shear hog to be precise, but it is plowing right through a significant part of the tool. This has not happened until recently which is leading me to believe that something that defaulted differently in the past has changed--I recently reinstalled Mastercam after upgrading operating system and RAM on my computer to Win 7 Professional (64). Remember when at one time the default Tip Compensation changed from tip to Center? That bit me a couple times as well, as I use bullnose and ballmills often. On the fresh install of MCX5 MU1, I did notice that the Minimal Vertical Retract Output feed is checked, putting in feed moves rather than rapids on the retracts. I'm wondering if unchecking this could lead to this issue. Also below this in the Linking Parameters is "Fitting". It defaults to Minimize Trimming. What exactly is going on here? Could this have anything to do with this gouging problem? What's baffling me is that Verify does not catch the gouges.

[Oscar R.]

"I have seen the tool rapid through the part with Optirough and Hybrid, but never with HST Core Rough if you feed the tool. I believe Bruce was only describing the issue with HST Core Rough."

 

Ahh yes, I see. Sorry, I mis-read.

[peon]

Unchecking that box is the issue Bruce. Minimize Trimming should have nothing to do with it. I made that mistake once when we bought our first HAAS. HAAS will dogleg the rapid move, unlike the other machinery we had in our shop. Verify WILL NOT display that rapid move.

[Bruce Kanzelmeyer]

When I check the Output feed move box and post out the tool path, I get the same error. I can see in the code the exact point where the Z does not retract to a level that clears the part. It seems to be retracting incrementally from the cutting level at the first retract that must clear the part. The following retracts are then correct and do clear the part, until we get to the next cutting level. Then, at the first time that the tool must lift to clear the part, it retracts to a point incrementally above the cutting plane (deeper than the previous time), and then gouges through the part again. Subsequently the lifts are correct until we get to the next cutting level. So far, the only way I can prevent this from happening is to use Full Vertical Retract. Any additional thoughts would be greatly appreciated. This definitely was NOT happening before I reinstalled Mastercam this last time. Thanks.

[peon]

Can you post a zip2go onto the server? We can take a look at that.

[Bruce Kanzelmeyer]

I posted 480-24397_2up_tool.z2g in X5 files folder on the ftp site. Sorry, it's a pretty large file. I've never used that utility before, it seems to throw everything including the kitchen sink into the file. If you scroll down in the 480-24397_2up_tool_test.nc file (which uses feed retracts--output feed move box checked) to Z-0.8918 machining level (about 1/3 way down), you will notice the passes retracting to Z-.6774 for several passes until it gets to the retract Z-.1658. This following XY move goes right through the part. On the following pass, the retract goes to Z.2573. This is correct, and misses the part. You can also notice this in the 480-24397_2up_tool_top.nc file that was my original with rapid retracts. What is strange is that this just started happening. I have been using this machining strategy using rapid retracts for many years without this problem.

 

Thanks!

[peon]

I'll take a look at it when I get a few minutes bruce. I prefer the zip2go with everything rather than just the part file.

[peon]

Bruce, do you see the issue while backplotting? I'm backplotting the part and analyzing the z levels you mentioned, but don't see an issue. I wonder if something is jacked in your post.

[Pilot Plant Supervisor]

I had a similar problem. Mine was retracting and feeding across the top (Z zero) even though that stock had already been removed. I solved my issue by changing the "keep tool down" distance to a small value. For some reason it defaults to a large value on my system.

[Bruce Kanzelmeyer]

Peon, thanks for your efforts. I'm thinking now that it is the Haas doing something weird in the rapids. It's funny that I haven't noticed this issue before--maybe I just hadn't paid attention to the fact the I have been using feeds box checked! It sure seems like I would save time going with rapids, but obviously the machine doesn't interpret the straight lines correctly in rapid mode.

 

Again, thanks for your help.

[peon]

I noticed when I looked at your part that it was a HAAS. The HAAS machining centers always rapid with a dogleg rather than a straight move. I couldn't post your toolpath with your post because I don't have a license for the router. Yes Pilot, if you have too small of a "Keep tool down within" value, the damn tool will drag across the top of your part simulating a gouge. Very frustrating! You can also lessen your chances of that dumb move by NOT using the "minimum distance" retract option.