Solidworks > STL > VCarve Pro 9.012: Artefacts

[JFDuval]

Hi all,

I recently bought a Stepcraft (2-840) and VCarve Pro. I have no problem with my 2D or 2.5D projects, but I’m struggling with the 3D ones.

All my design are done in Solidworks 2017. I’ve been exporting my files as STL. When I import them in VCarve, I get “artefacts” near some features. As a result, I’m getting bumps where I should be getting straight lines, and the endmill doesn’t go in certain spots because the software think there isn’t enough room.

First, here’s my test part (for the curious, it’s a hand plane shooting board that will be used to joint wood) in SW:

Solidworks PNG

And here it is once imported in VCarve. I’ve highlighted the most problematic zones:

VCarve PNG

The STL and the VCarve files are available: https://www.dropbox.com/sh/swxlzeeapel2 ... xHGBa?dl=0

Things I’ve tried:
- I imported the same STL file in Solidworks: it looks good, no bumps. I also tried https://www.viewstl.com/: no problems.
- I’ve tried increasing the resolution to the maximum available: no difference.
- I’ve saved the same model as a WRL file: same issue.

This design can clearly be made in 2.5D, and that’s what I did to complete the project (imported a DXF, used a few different layers to get the different depths). However, I have other projects that require complex 3D surfaces so I’d like to find a good solution.
Have you seen this problem before? How did you solve it?

Thanks have a great weekend,

JF

[martin54]

Not an expert but from other posts I have read on the forum it may have something to do with vertical edges, try a search on the forum as there have been a number of posts about this sort of thing

[LittleGreyMan]

Hi,

This part is clearly a 2.5D job, so exporting to dxf is the better solution.

We recently had a problem with a Solidworks 3D part. It was OK within Solidworks, but the STEP and IGES exports were distorted in several zones with every other software we used: several CAD and CAM systems, including high-end software. Re-importing them in SW was OK. Unfortunately, as we had to machine the part, it gave us a lot of repairing work in another CAD system before being able to export it for the CAM software.

Can you post the original SW file? I'll give it a try.

[Leo]

I am a solidworks guy myself. I am also a Vectric guy.

Doing that file in an STL or any 3D model format is not a good choice.

If I were to do that job it would be purely Vectric and no 3D model at all.

It's not worth the effort to try to solve the Solidworks - STL - 3D model issue.

There is a place for a 3D model, and Solidworks does work well with STL export. That one is not one that will work well.

[JFDuval]

Hi all,

I attached the Solidworks file to this post. While this part is simple, most of what I want to do with this CNC isn't; re-designing the parts in Vectric is out of the question.

Just to be clear, we use STL exports for a lot of 3D printing, and for some machining shops. We've never had such a problem.

I'll so a search for vertical edges and let you know if I find a solution.

Thanks, JF

[Adrian]

VCarve is pixel based which can lead to issues with vertical sides that you won't see in other packages. That doesn't mean you will see issues with parts more suited to 3D work than the shooting board.

The usual "fix" is to machine the vertical sides with a 2D profile cut.

[garylmast]

I have the AutoDesk Suite 2013 which includes Autodesk 3Ds Max. Too many times I had issues when exporting as a stl file, parts of the drawing would be all over the place. Vectric won't recognize 3Ds Max files and also had issues when I exported them as a DXF. I use Rhino almost exclusively how and don't have any problems. Vectric allows Rhino files to be imported, maybe in the future they will include other file formats. It wasn't only Vectric where I was having problems, my Laser Engraver uses DXF files and too many times there was an import issue when came from Autodesk 3Ds Max.

Gary

[LittleGreyMan]

I attached the Solidworks file to this post.

I don't see your file. You may need to zip it.

While this part is simple, most of what I want to do with this CNC isn't; re-designing the parts in Vectric is out of the question.

Machining this kind of part with 3D toolpath does not make sense, as Leo and I mentioned. Machining and finishing time will be much higher than with 2,5D toolpath.

[JFDuval]

Hi all,

I prepared a new Solidworks test part that can't be cut in 2 or 2.5D. It's designed to be machined with a 1/4in endmill (smallest radius: 3.5mm). The part is 100x100x25mm. The bottom is 5mm thick (deepest cut: 20mm). The narrow channels are 6.4mm, just wide enough for a 1/4in tool.

Exported as an STL with the highest resolution possible (big file, 17MB). The file is available here: https://www.dropbox.com/s/usw32xuswsrkh ... 1.zip?dl=0 (too big for the forum even when zipped). Looks fine once imported in VCarve:

First toolpath: rough machining, 1/4 endmill, 40% stepover, pass depth of 0.125in (3.175mm), model boundary with boundary offset of 7mm, 0mm machining allowance.

Q1) Why is there material left at the bottom of the channels? The walls are vertical, and the clearance is wider than the tool diameter.

I tried adding a Finishing pass. Same 1/4in endmill, 10% stepover. It didn't remove the extra material:

Using a ballnose instead gives me a nicer finish on the top of the part, but I still have the same problem at the bottom. Plus, because the Rough pass didn't go all the way to the bottom I now have rounded egdes:

My VCarve file is attached. What mistake am I doing? Is it an issue with my STL import, as I initially suspected, or am I doing something wrong when I'm calculating the profiles?

Thanks, JF

[Leo]

The general rule of thumb is to use the largest tool possible to do the job. The issue I see in that doing that part with one cutter as a 3D part will makes the cutter quite small, so it can fit into the small areas.

There is an issue with 3D and near vertical side walls. The step over value is an "X"-"Y" axis move, therefore and "X"-"Y" move on a side wall will manifest itself to be a HUGE "Z" move. In order to overcome that issue the stepover needs to be extremely small - like .0001 and that is not a decimal point error. On a 45 degree angle or less the stepover is not as critical.

You CAN create vectors to isolate boundary areas and use different cutters with different cutting parameters. This does NOT need to be done all in one shot.

[JFDuval]

Hi Leo,

Thanks for the explanation. Now I see how a small pixel error on a side wall can lead to big un-machined areas. Now... what's the best way to work around that? I tried with a 1/4in endmill and a very small stepover (0.0001in). It took my computer 15 minutes to generate a toolpath and a preview. It has the same problems, and it would take 94h (!) to machine.

I've been exchanging emails with tech support too. Their solution is to use a mix of 2D and 3D, and/or to use a smaller tool. I can do that, but that seems hacky and it will be time consuming for bigger projects. I'm also worried that I'll miss some features that the 3D path is skipping and that I'll get parts that do not work. Is that what you do for 3D projects? Or do you use other CAM software?

Thanks, JF

[Leo]

I agree with a mix of 2D and 3D.

If I were going to program that part in my Mori Seiki Vertical Machining center with MasterCAM I would be using 2 or 3 or 4 different cutters.

In MasterCAM I would create boundaries and I would program the cutters to do the cuts I need. Those would be the sharp square inside corners and flat bottoms and tops. I would create boundaries and use 3D patterns and ball nose cutters for the areas that I cannot use 2D cutters and operations for. That is all in a professional industrial manufacturing atmosphere. I would not do that as a 3D part in my job. It is just not efficient.

In Vectric you can do something similar with vector boundaries, and separate the areas you want to focus on.

As a test to see what I am talking about - take your STL and just draw a circle on it - anywhere - it doesn't matter where - this is just a test - make the circle to about a 1/4 of the part. Now - use your 1/4 end mill and to a finish 3D but select the circle. Calculate. The only machining done is inside the circle. In this way, you can draw vector boundaries and isolate any area with a boundary vector. You can draw vector boundaries to create pocket areas to do the 2D work.

The vertical walls I was talking about has nothing to do with pixels at all.

[Adrian]

Why such a big boundary offset on the roughing toolpath and no boundary offset on the finishing toolpath? Usually I have both set the tool radius to ensure that the software doesn't see the bit catching on the side walls as the toolpaths are calculated from the centre of the bit.

These videos are well worth watching to see the most efficient methods of 3D machining -

http://support.vectric.com/tutorials/V8 ... g3D_1.html
http://support.vectric.com/tutorials/V8 ... g3D_2.html
http://support.vectric.com/tutorials/V8 ... g3D_3.html

[mtylerfl]

Absolutely agree combining 2D and 3D to achieve the desired outcome. I do it often.

For example, I may carve a 3D item with a 7degree tapered 1/16" ballnose bit. This can leave a "chattered" angled edge where I want a nice neat vertical wall. In that case, I'll use an appropriate straight end mill to remove the angle and leave behind a neat vertical wall. Very common procedure and nothing out of the ordinary for that.