Help! Outline offset relative to drill locations in single setup... A head-scratcher.

[wesg]

Can you mirror the toolpath in f360?

Rather than mirror the part in CAD and program each separately, program 1 climb and conventional, and mirror the conventional to climb the other part.

I did some big molds this way in surfcam, rather than managing 2 CAM files or a bunch of layers for the mirrored parts. Of course I wound up with 3x the number of operations to manage.

 

[13engines]

On a little closer look at your original Fusion screen shot, I'm thinking that those millions of blue lines are representing the tool path of the main cutter used create the shape of your parts. Man that is a ton of tool path. So much so that I'm thinking out loud these ideas...

1) You have some kind of stacking error due to the immense amount of back and forth movement of the ballscrews. 0.0001" error in backlash comp or the likes added up a couple thousand times equals something that looks like an error. It doesn't show itself as much in the drilled holes which are practically single movements. (Number 1 here seems doubtful but...)

2) If not that then the effects of that in the way of heat. Whether in the material and/or the ballscrews. Have you tried doing all the drilling first and running one half in the morning, then letting the machine and stock cool back down completely, and running the 2nd half the next day or after say half a day of cool down? Not practical for production of course but may serve for investigative purposes. Wonder what the coefficient of thermal expansion of this material is?

3) What if you took the 2nd part and rotated it 180 degrees around Z so it faces in generally the same direction as the mating part. That way if you're getting growth it will be applied equally on the handle. Meaning blade end done last in both halves instead of first in one and last in the other. This assumes the tool is for the most part, progressing continually along one axis from one end of the fixture to the other. This also assumes the growth is continuous throughout the run. I imagine you could do this program wise, but that would change one variable, as in the main direction the machine is moving during the cut(s) from one half to the other.

Heat growth or stacking error or both. Maybe?

 

[aarongough]

Can you mirror the toolpath in f360?

Rather than mirror the part in CAD and program each separately, program 1 climb and conventional, and mirror the conventional to climb the other part.

I did some big molds this way in surfcam, rather than managing 2 CAM files or a bunch of layers for the mirrored parts. Of course I wound up with 3x the number of operations to manage.

Interesting suggestion! I had to look around to check on that as I have never tried to mirror a toolpath. Turns out the answer is no in Fusion. You can mirror parts but not toolpaths, every toolpath is associated directly with CAD geometry.

 

[aarongough]

They aren't. If they were, there'd be no shift. Somehow, in the flop, things are getting moved. Or the fixture is wrong.

Your fixture method is similar to what lots of people do for horizontals, but many people will put the tombstone at a fixed point, like you, then each part will have an offset so that the individual programs can be written from a feature on the part itself. You are sort of doing this in the 1970 NC method. It works but harder to troubleshoot, imo.

How about trying it raw, instead of mirrored ? Make a completely separate pair of programs .... it's more likely that fusion has a bug than the control.

Have you checked physically to see that the fixture is correct ? Indicate your locating features and make sure they really are where they are supposed to be ? Double-check the math on those locations ?

Hey mate, I think there's some stuff you've missed. Read through my post above regarding the position of the fixture/stock/offset. If any of those were out of whack by 0.01" (or even more) in X or Y it would have no effect on the dimensions of the finished part.

Also: I have definitely checked the gcode itself for symmetry. If you have a look at the second image in my first post you can see data from a gcode backplotter... Not Fusion, another program that's taken the generated gcode and then read it back in so I can verify that the dimensions are correct.

 

[aarongough]

ISSUE SOLVED! Hooray!

Ok, so this morning I moved the parts in CAD the tiny bit needed to make them perfectly symmetric around the Y axis origin:

Here is a sketch showing the models are symmetrical around the origin:


And here is a backplot of the gcode output with coordinates showing that the parts are mirror images of each other:


Unfortunately this did not solve the problem. In my mind this is actually a good thing... It would have been very unintuitive if this solved the issue

Ok so onto the next item: changing all the tools.

I did this one as kind of just a 'belt and braces' item because the tools were still producing good finishes and drilling to size and so on. I wasn't really expecting it to fix the issue, and yet IT DID!?

Looking at the part and program I think I know why. As G00 Proto suggested I think it was drill bit wander.

I think of G10 as a pretty soft material (which it is) but it also is pretty good at dulling tools. The drill bit I was using was a screw machine length solid carbide drill held in an ER collet so it should be pretty stiff, but it had been in there a long time because I'd never had any reason to change it...

I think the drill was pulling/walking off position just as it started the hole. I have never had this issue before so didn't really think to look for it. I have changed the program so the counter-bore happens first to ensure a perfectly flat starting spot for the drill, and I will make sure to change that drill more regularly!

In the end it was definitely a head-slapper. I discounted a potential problem because I 'ass-umed' it could not affect the part the way I was seeing... Lesson learnt!

Thanks to all for the feedback and ideas!

 

[Bobw]

Don't you hate it when its something stupid. Bang your
head against the wall for days, and its the thing you
completely discounted right at the beginning, because
"NAH, It could never be that.".

Now the question is.. Why did it only wander in the Y direction?

Too much tool pressure lifting your head up?

Maybe flip one of the parts 180 degrees, so if this problem
creeps in again, the wander will be in the same direction,
and the two sides will line up.

 

[mutiny]

Great to hear it's solved! Were you drilling into a curved surface? If so, I'd sort of expect some amount of variance from that just based on the position of rotation and how the first flute catches the material. Spotting the drill location may give you some better process reliability even if you don't need it with fresh drills.

 

[Bobw]

Great to hear it's solved! Were you drilling into a curved surface? If so, I'd sort of expect some amount of variance from that just based on the position of rotation and how the first flute catches the material. Spotting the drill location may give you some better process reliability even if you don't need it with fresh drills.

Why spot? If you need a spot, especially with a carbide drill, just use the drill as the spotter.
Run one drill cycle at a low feed and low depth, and then come back and punch it. I wouldn't
do it with a long chisel point, but it works pretty well with split points, even jobber length.

And it saves a tool change, and as we all know, on a Fadal that takes FOREVER!!!

 

[mutiny]

Why spot? If you need a spot, especially with a carbide drill, just use the drill as the spotter.
Run one drill cycle at a low feed and low depth, and then come back and punch it. I wouldn't
do it with a long chisel point, but it works pretty well with split points, even jobber length.

And it saves a tool change, and as we all know, on a Fadal that takes FOREVER!!!

Fair enough!

 

[aarongough]

Great to hear it's solved! Were you drilling into a curved surface? If so, I'd sort of expect some amount of variance from that just based on the position of rotation and how the first flute catches the material. Spotting the drill location may give you some better process reliability even if you don't need it with fresh drills.

Yes the starting surface was slightly curved which I definitely think made the problem worse... I think I actually previously traded one problem for another. Months ago I found the scale outlines didn't line up but it was less bad and also less consistent. At that point I realized I was drilling the pin holes before performing the roughing operations, and I think the stock was moving.

To solved that I moved the drilling operation to after the roughing operations were done, but that meant I was now drilling on a slightly curved surface!

Fixing one problem and making another!

 

[G00 Proto]

Yes the starting surface was slightly curved which I definitely think made the problem worse... I think I actually previously traded one problem for another. Months ago I found the scale outlines didn't line up but it was less bad and also less consistent. At that point I realized I was drilling the pin holes before performing the roughing operations, and I think the stock was moving.

To solved that I moved the drilling operation to after the roughing operations were done, but that meant I was now drilling on a slightly curved surface!

Fixing one problem and making another!

We drill about 400,000 3/4" deep holes in G10 like material every year. The holes don't like to be straight, the correct diameter or on location... other than that, they are usually right.

Drop the counterbore in first, then helically bore to ~.050 below the pointy part of the drill (I think that is called the margin or maybe the shoulder... you know, the pointy part). That will make sure that it is located correctly to start. It shouldn't wander too far from that. Stub length Guhring two flute carbide drills. Talk to them about speeds and feeds, they have strong opinions.