Convert to 5-axis - gouging

[Bob W.]

I am machining a narrow channel with steep walls that needs to be done in 5-axis to provide tool clearance to the walls. This feature is shaped like a hook as viewed from the spindle. I created a blend 3-axis toolpath that pretty much acts like a 2D HST peel mill toolpath and then converted to 5-axis to get exactly what I am looking for. In Mastercam backplot and verify the toolpath is perfect. The problem is, when this is posted and run through Vericut there are some wild C-axis moves that are causing gouges. These are not shown in Mastercam backplot or verify. I have tried everything I can think of from the misc integer settings on the primary and secondary axis constraints etc... It appears that the issue arises when the tool goes from a slight lead to a slight lag, the C-axis does a 360 degree rotation. This is well away from the B or C-axis centerline, about 3-4" from the center of the rotary table. Any ideas? Post settings I should look into? This is on a Makino horizontal machine with a rotary table.

[gcode]

is it happening as one axis approaches 0 degrees?

you could try breaking it up into 2 tool paths

you could also try rolling the toolplane of the 3X

blend tool path a couple of degrees

[Jim at Gentex]

It appears that the issue arises when the tool goes from a slight lead to a slight lag, the C-axis does a 360 degree rotation. This is well away from the B or C-axis centerline, about 3-4" from the center of the rotary table.

 

I've seen this happen using lead / lag, especially when trying to transition from one to the other in the same toolpath.

It's not so much that the toolpath encounters a B or C axis centerline dilemma, but a positive to vertical (zero) to negative dilemma.

I think when your post encounters that vertical zero condition when transitioning from lead to lag it is throwing that C move to try to deal with it. (Convert to 5 axis in general adds an extra layer of complexity for your post as it is.)

 

I've used gcode's idea of breaking it into 2 separate paths at the point where it goes from lead to lag or vice versa and that usually works.

There is probably something in your post that controls that movement, but if you are pressed for time it may be simpler to just break it into two separate toolpaths.

 

Unless one of the post gurus here can tell you exactly where to look, I would try the simple fix first.

[Bob W.]

I do believe it is a lead/lag issue for sure. I'll try breaking up the toolpath a to see how that goes.

[Zoober]

Maybe check fanning distance?

If it's too large, it may be trying to reposition instead of fanning

[gcode]

what are your tool axis control settings

it sounds like you'd want to use a chain centered on the

groove

[Bob W.]

Fanning is set to .05 and the tool axis control is set how Gcode described, a curve down the centerline of the groove with the tool axis at the nearest point or start to finish. I have tried both.

[Bob W.]

Looks like I got it solved. I broke it into two toolpaths, switched to 'from start to finish' on the tool axis control and adjusted the start and end points of the contours to keep the tool in a leading posture. Thanks a ton for the insight it was a huge help!

[Jim at Gentex]

Glad to hear it!

 

This place is a gold mine of experience.

I've found that almost any problem I've encountered with a 5 axis programming job, someone else here has had it and can help solve it.

[gcode]

that's the nice thing about the Moduleworks addons.

There are usually dozens of ways to approach a problem and one of them is bound to work

[metalmansteve]

So is the moral of this story to never attempt 5- Axis programming without vericut? Sounds like it paid for itself with this one job.

[Bob W.]

Yep, I literally ran a dozen simulations where the posted program failed to various degrees. The minimum was scrapping the mold half, then there were the issues that would have scrapped my $4000 air spindle AND the mold half, then there were the full machine crashes that would have damaged the spindle and rotary table. These were all on a program that looked perfect in Mastercam. When I did finally get a program that worked in Vericut I loaded on the machine, hit cycle start, and went to bed. The machine finished up at about 8:00am and the program ran fine. That is my confidence level with Vericut's results.

[gcode]

Yep, I literally ran a dozen simulations where the posted program failed to various degrees. The minimum was scrapping the mold half, then there were the issues that would have scrapped my $4000 air spindle AND the mold half, then there were the full machine crashes that would have damaged the spindle and rotary table. These were all on a program that looked perfect in Mastercam. When I did finally get a program that worked in Vericut I loaded on the machine, hit cycle start, and went to bed. The machine finished up at about 8:00am and the program ran fine. That is my confidence level with Vericut's results.

 

In my experience with a 5X head/head machines, posted code = verify backplot to the point that I rarely use Vericut.

 

With the 5X horizontal trunnion machine we bought last year, its a completely different story.

 

 

The angular limits of the A axis add a whole new level of trouble to the mix.

Wild and unexpected rotary motion are a regular occurrence.

 

I ran it for about 3 months without Vericut doing full 5axis vane work and it was very stressful.

I would post one operation at a time, run it through CimoEdit backplot, do text searches for

sudden changes in A or B values etc etc..

It was very time consuming, dangerous and nerve racking.

We never solved the wind up/unwind issues with Mastercam posts and I ended up

buying a post from ICAM.

It is much better, but far from bulletproof.

 

I have a professionally built Vericut machine for our 5X HMC now, and

I run all code through it before it goes to the machine.

It has saved me from several catastrophic crashes easily justifying it's purchase cost.

[Zoffen]

Ya vericut really cuts down on the stress with 5ax stuff, or just programming in general.

love it, wouldn't work without it now that i have it.

[Mick]

So is the moral of this story to never attempt 5- Axis programming without vericut? Sounds like it paid for itself with this one job.

 

My experience is exactly that. I wont run any programme on our 5 axis machine without putting the code through Vericut. I built our machine model for Vericut (Okuma MU500VAII), and it has proved its worth over and over again. It has paid for itself by picking up potential errors.

 

It is also great to be able to try different cut strategies without tying up the machines resources.