Here is an example of what I'm trying to do:
Imagine 10" diameter by 1" tall raw material. We are milling a 9 inch diameter x 1" tall cylinder from raw material. The tool is a 1" insert cutter and we will be cutting with a 0.5" step over and a 0.1" Z increment. I would like to machine the part in such a way that the tool does the necessary 10 x 0.1" steps down before it does each step over. Meaning, axial steps before radial steps.
One way that the engineers I work with now take care of this is to generate a "profile" operation for each step-over. This seems archaic to me.
Does anyone have an effective, secure, and relatively simple method of doing this?
You're help is appreciated!
Assuming the walls are vertical, use profile_3d for wireframe, or solid_profile_3d if you have a solid body. Go to cutting parameters, multiple passes, set your side and depth passes, and set the order to depth first.
At first, I tried this and noticed that the paths where ignoring my blank. I adjusted this by adding a trim boundary based on my stock size:
I set up an example using a block for my blank and a cylinder (9" x 1"D) for my part. I made the edge of the block my trim boundary and selected the wall of my cylinder diameter for the wall. Using "Solid Profile 3D" with "multiple passes" and "depth first" seems to have worked really well, initially. The one things that I can't seem to overcome at the moment is the trim boundary is clipping from the center of the tool rather than the cutting edge. Is this something I can change or do I need to create a new boundary?
Ultimately, I don't understand why I can't do this with a profile pass. "depth first" seems to have no effect on that operation. This, using solid profile 3d, seems like a compelx workaround, of which there are others that may be simpler. Suggestions, updates, ideas?
Thats depressing. Where can we add our voice to the storm? I've used some of the lamest, least powerful software out there, and its had the this capability. I wouldn't ever go back to it, because NX's capabilities go way beyond this one fault, but **bleep**, something so simple...
Thanks for the help guys.
Where can we add our voice to the storm?
Open an enhancement request at GTAC and the customer count will be increased, so it is more likely to get included.
Production: NX10.0.3, VERICUT 8.1, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 11.4
Development: C (ITK), .NET, Tcl/Tk Testing: NX12.0 | AWC 3.4 Preparing: NX12.0
Employees of the customers, together we are strong
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide
Trim boundaries by design trim the tool path - this is why the tool is "on" and not "tanto".
We have enhanced the offset in custom data, so that you can specify %Tool, which should provide what you need:
This is complete and should be released soon.
Regarding Depth first in a single region...
The master ER for this is 6062801 for those that want to voice their desire with GTAC.
We have looked at this before, and it is easy if and only if the cut pattern at all levels is identical. So if all walls are vertical, and there is no collision avoidance, it is possible. But what would you expect if the pattern at each level was different? How would the system go "down" if the cut below is in a different place?
This is why we support it in processors that are based on straight walls. For vertical walls, this is profile 3d and solid profile 3d. In these cases, we know that the level below will have the same pass, so we offer the option.
If the walls are straight but tapered, then I would use contour profile, which also has options for multiple side passes, multiple depths, and the order in which they are cut - depth first or side first.
If you find that the only way to get what you want is with multiple cavity milling operations, then consider making a geometry group template, with different side stock in each operation. It would still be a single create and generate, but you would get multiple operations at once.
I created a custom boundary that was offset by the radius of my tool from my blank geometry. Now, the result is the path functions as if there is no trim boundary at all.
I get the same result if I modify my blank to be oversize by the radius of the tool, effectively modifying the trim boundary the same as above.
Does this imply that the distance of the trim boundary from the part determines the functionality of the trim boundaries? So modifying my trim boundary to allow my tool to fully profile the part in solid profile 3d results in no triming of the tool path at all. Once the trim boundary is contracted enough to allow effecient milling of overhanging material, I lose the path which fully profiles my part.
Thank you so for your input guys, I am being a little stubborn but I think it will be worth it in the long run for me to understand how this works.
Can post a 2D picture of what the part and blank look like, and what path you want?
If you are using boundaries, I suspect you just need to select the right boundary types - part, blank, check, trim.