How do you handle large CNC Projects (Large GCode files)

[Anonymous]

https://a360.co/2xMcMwI

I have this project that exports a 20MB GCode file (for use in xcarve) and its too big for UGS. Im a new user (to both Fusion and CNCing in general), how do you handle something like that.

[seth.madore]

That file is no joke!

I'd start by adjusting your tolerance and smoothing. Set them both to a larger value, leaving a little bit more stock. I'd also increase the size of your Minimum Stepdown, leaving more for a subsequent pass. 

What's the storage capacity of the UGS? I thought it could handle a lot more than that...

[johnswetz1982]

That looks symmetrical so you should only program one half them create a [Pattern] with a mirror in the Manufacture environment and post it out as 2 different operations. That should split your size in half. If you need to further reduce, split your design (one side) into 4 squares or something similar. Keep splitting until your at the files size you can handle. You can also try to turn on smoothing. that should reduce your files size.

[Anonymous]

yeah, without smoothing its 35MB. I'm trying to loosen the tolerances up a little and ill try the pattern thing. I have no idea yet how to do that.

[Anonymous]

Creating Identical Setups with Identical "Adaptive Cuts" with different boundaries? 

[johnswetz1982]

Go back into design. Create a mid plane down the center of your part. Back to Manufacture. Under setup select pattern. You should choose mirror and the midplane previously created. That will create a folder. Do one side of your design and drag that operation under the pattern folder. That will flip your design to be symmetrical. That way you don't have to worry about updating one side of the design and not doing the same on the other. 

[daniel_lyall]

you can do one side at a time from the model as it is.

What I would do and do is use a big tool to start with then go with a smaller tool then smaller tool again and or do a parallel toolpath to finish, this way you will have smaller tool paths.

You could use say 1/2in then 1/4in then 1/8in cutters to rough it out then when you go to finish it use a ball nose if you use a conical ball noses tool like this https://www.toolstoday.com/ball-nose-conical-ball-solid-carbide-spiral-cnc-2d3d-carving-tapered-and-...

you can cut a bit more of a depth of cut and width of cut and just cut faster. 

[engineguy]

@Anonymous 

Have you tried just "drip feeding" it ?? By far the easiest way, doesn`t matter what size the file is then 🙂 🙂

[Anonymous]

here is my attempt:

https://a360.co/2xMcMwI

It has toolpaths where it shoudnt. Im sure i screwed up somewhere. It also take 4-5 hours for my 5GHz machine to create the toolpaths... 

I have also tried parallel, but that makes it take about 1/32 off that it shouldnt either. (I definitely probed the z axis and the piece is flat)

[daniel_lyall]

What tool did you use for the parallel toolpath?

[johnswetz1982 · Accepted solution]

See the linked, You only do one side and the pattern mirrors it for you. Click on the Folder then the individual operation to see the difference. You should try to rough it out before you try parallel. If it cut too much and you zeroed correctly perhaps the bit pulled out from too much force.

Check the feeds and speeds as I left them default. You had your tolerances way too tight for an art piece so I open them up. You final file will be much smaller.

https://a360.co/3deetmH 

[Anonymous]

Thank you!

I went back in and did the same things you did (to learn) and the 1st file was about 1M(adaptive). and the 2nd was 700k(parallel)