Part envelope violation using z-level profile

[DaSalo]

Using 7.5.3.3:

I have some parts that are basically shaped like a wedge. We are milling these in a vertical orientation (thin end of wedge pointing straight up) by spiraling down the shape from peak to base using z-level profile. I have the in/out tol set at .0002/.0002 and a .0002 scallop height. Looking at the surface in the finished part it is clear that there is a very small amount of negative geometry right up at the tip of the wedge (the tip curles over a small amount) and the side of the cutter is hitting a bit. I see no indication of this at all in the NX cutter path. No gouges or collisions are detected in verify. Am I missing a tolerance setting somewhere? Is there a way to 100% reliably detect negative geometry no matter how small?

We can cut these parts with a lollipop cutter to avoid the issue but I would like to understand how to identify this situation at the programming stage before the parts get cut.

Thanks for any help.

-Jeff

 

[DaSalo]

No bites the first time around so I'm going to try to clarify my question a bit:

- How does NX verify define a collision or a gouge?
- Is it any violation of the stock envelope or is there a tolerance that applies to this?
- If there is a tolerance is it the in/out tolerance in cutting parameters or is it elsewhere?

- Does Z-Level Profile, or any other contouring operation type, check for undercutting? I know there is an an explicit check-box to allow/disallow in planar operations but nothing that I can find in contouring operations.

Hopefully someone can straighten me out here.

Thanks for any help.

-Jeff

 

[capnhook]

Z-level profile and its cousin cavity mill have always had problems with gouging. Cavity mill also has a problem with small areas not being recognized, and therefore them being left uncut. There must be a list if IR's a mile long on these subjects, but I never hear anything encouraging about this code being fixed. The attitude I got from GTAC was, "We can see there is a problem, but you're on your own, buddy. It is not on our priority list."

A person can get real good at hand editing programs, and in this case, has to.

capn

Proud Member of the Reality-Based Community..

 

[DaSalo]

I'm sorry to hear this. I was hoping I was missing a setting somewhere. The toolpath that I am getting is odd, it gouges a bit here, leaves some stock there. It generally seems to be trying to take the best average of gouge/excess but it favors excess a bit. I am very surprised to learn that the in/out tolerances do not hold absolutely.

This makes me loose a significant amount of confidence in NX CAM. If you give me a box to set tolerances and I fill the box with valid values I expect those tolerances to be respected absolutely and an error message, skipped area, or something similar to result if the path is not able to calculate within those tolerances.

 

[DaSalo]

Is there another type of operation that I can use that is better about avoiding gouging that can be configured to give a spiraling type toolpath where the cutter enters at the top of the part and smoothly ramps down to the bottom? I have Z-level profile set with "stagger ramp on part" stepover so I get a continuous path but it isn't a continuous ramp. A continuous ramp would be even better, especially if it would avoid undercutting.

 

[capnhook]

I have used Brand "C" software, and have built the kind of path you are describing. I have seen demos of Brand "M" software handle this brilliantly. You may have to switch to another CAM software to do what you need to do.

There does not seem to be an emphasis or priority for this software manufacturer to correct its obvious "misteaks" in this code. I would be happily surprised that this was repaired in the new NX8 release, although I am not anticipating anything being done to fix it.

Sometimes, one has to stop trying to push a rope up a hill, so to speak, and try another product.

Proud Member of the Reality-Based Community..

 

[markrief]

Before you make any decisons, please contact GTAC about this, or inquire through the Siemens support channels.

If you are spiraling down with zlevel, I assume you are using either the engage or the ramps between levels. You may be better off with surface contouring with streamline drive.



Mark Rief
Product Manager
Siemens PLM

 

[DaSalo]

I'm not even close to jumping ship on NX, this is not even close to that big of a deal. NX CAM has been absolutely reliable for me up to now and, as I mentioned above, a change in cutter type allowed to us to run these parts without any trouble.

I will contact GTAC to try to understand the issue more clearly. I have no problem with the software having limitations, I just would like it to notify me when I have hit them instead of fudging the path, which is what it seems is happening here.

I'll try streamline drive. I've never used that option so it might be the better approach for the job. If so, we can chalk this up to driver error.

 

[capnhook]

Perhaps most users have the luxury of waiting days for an answer from GTAC, that there is something wrong with these types of operations, and that there is no priority to fix the code.

I do not have that luxury. I have to either hand-edit the operation, or use another program.

When you (soon) happen to run into the new Streamline operation bombimg when machining in an assembly, please let me know. I have a work-around for that.

Proud Member of the Reality-Based Community..

 

[DaSalo]

Well I was able to kind of get a spiral path on this thing using streamline but the path is terrible quality. Tons of jigs, jags, and bumps. I have been told by a colleague here that streamline and surface area operations are looking for clean surface bands in the direction that you are trying to cut. I don't have that and am not going to get that without some seriously involved reworking of the part.

Z-level profile works great. It gives me a nice smooth path just like I want. Only problem, that I have recently discovered, is that it really doesn't recognize the added clearance in the toolshank that you get from a lollipop or barrel type cutter. I though it was giving me a better path with the lollipop but on closer examination the path was identical and the particular part I ran with the lollipop just had less negative geometry than the others I was looking at. The path still leaves excess stock in the hollows even though the cutter is perfectly able to get into them.

So now the question is: Is there any operation that will behave like z-level that can recognize and take advantage of the extra clearance in the lollipop? I have also tried area milling and that gives me the same problems as z-level.

Attached is an image from a path created in area milling that shows a subtle wrinkle in the toolpath right over one of the areas with a bit of negative geometry. The crest of that wrinkle is about .004 excess stock. We can tolerate .001 or so but not much more.