solidworks stl issue? could use help.

[shaun]

I created a file in solidworks and saved as an stl. I imported it into partworks 3d and created a tool path. When I run the file the first pass seems to cut ok but when it steps down to make the next pass the machine stutters and looses its x and y zero. I end up cutting that path offset unless I am standing there and stop the machine.
I was thinking I had a mechanical issue but I think it is software. I created a similar file using partworks. just a big hole cut in a block and it ran fine. When I did it in solidworks and tried it I had the same problem. Definately gets confused trying to run the tool path created from an stl import.
Anybody have any solutions?
I have version 1.002 of partworks 3d and version 10 fo solidworks.
regards
Shaun

[Brady Watson]

What are your move speeds/cutting speeds set at when cutting the STL?

Under VR, what is your XYMove Speed? ZMove Speed? Slow Corner Speed?

-B

[shaun]

Brady,
I chose 3 inches per sec for feedrate and 2 inches per second for plunge.
The VR xyMove speed is .4
The ZMove Speed is .4
move ramp rate is .15
slow corner speed is 65
3d ramp threshold is 100
regards,
Shaun

[Brady Watson]

move ramp rate is .15 -- Change to .2
slow corner speed is 65 -- Change to 45
3d ramp threshold is 100 -- Change to 150
Min Distance to check -- Change to .08

What are the overall dimensions of the carving in XY and Z/depth?

Also - Did you create & run a roughing pass with a square end tool before running a finishing pass with a ball end tool?

-B

[shaun]

Ok, will try cutting it tomorrow.
The actual job is 10 x 18 x 3. I was planning on cutting it in foam to see if anything hits.
The practice piece is a 4 x 4 x 1 block with a 3 inch hole 3/4 deep.
I actually used a 1/8 ball nose for both. Should my roughing be a 1/4 mill?
shaun

[Brady Watson]

You should run a roughing pass on it & reduce your cutting speed. Using the same file, start cutting at 2,1. See how it goes. If you feel that it is OK, increase the speed. That's a lot of material for the finishing tool to hog out in one shot.

Unless the relief is only like 1/4" deep, you should always do a roughing pass. Try a 1/2" for roughing and see how much material the 1/8" has to take off. If there are big chunks that the 1/2" misses, then use the 1/4.

The idea behind roughing is to get all the big stuff out of the way so that the finish/3D pass only has to shave off a little bit of material. This reduces or eliminates cutter deflection and tool breakage. If you have never done a roughing pass before, Vectric and DelCAM leave by default .02" of 'meat' on the relief for the finishing pass to shave off.

Oh...make sure you leave a spot on your material to zero both your roughing tool and finishing tool. You should C2 at the same place.

-B

[shaun]

Brady,
I will definately need to read up on VR. It seems to have fixed the stutter and loosing zero. Unfortunatley, I seem to have a new issue. The file is not cutting as the preview shows. I am getting this very strange square tooth pattern around the outside and in the center. I tried doing a different post processor because preview looks good but same effect. Any ideas what I should look at?
shaun

[Brady Watson]

Post a pic or two so we can see what is going on.

-B

[shaun]

Brady,
The two pieces of foam represent the STL import file and one I created in partworks. The little piece is what the end result is supposed to look like.

[Brady Watson]

OK - the one with lines...what did you define your stepover value to be on the toolpath when you created it? Was it a roughing pass or finishing pass?

The part you have shown (finished) is a 2D part. If I were cutting it I would first do a pocket in the center, then do the outside profile - all with a regular 2-flute end mill or router bit.

-B

[shaun]

Brady,
I think you nailed it again. My step over was .625 instead of .0625. I did not conciously set it. I need to learn each of these functions better. I have probably never used that bit before and I obviously do not know what I am doing yet. I have been using the default settings on the bits. I will try cutting it again and see what happens but I think this should fix it. It was a roughing pass.
The finished part is exactly how I did it. Nice to know I somewhat think properly:)
It is a practice piece to see how difficult it would be to import files from Solidworks before I try something more difficult.
Thanks so much for the help.
Shaun

[Brady Watson]

No problem - Glad you got it sorted out. Keep practicing...you'll be humming right along in no time. It takes a while to learn how to 'think in CNC', and discern between what is a 3D part and what can be created with 2D strategies. If it can be done via 2D, then do it - it is always faster.

-B