Vcarve pro help please: Slow jerky cutting!

Hi,

I was hoping someone on here could help me, it would be much appreciated.

I am fairly new to CNCing. I have been using vcarve pro for 3D milling from 3D stl files created in Rhino. When i import the file into vcarve it converts to a pixelated model. I set the resolution to the highest setting (50X) but it is still pixelated.

The problem I am having is when I CNC the model the cutter moves very slow in jerky movement as it cuts around the pocket for the roughing toolpath on curves and some of the finishing toolpath. Even with the feed rate at 430mm/sec. The straight cuts are fast. I assume its because the CNC is reading the jagged edges of the pixelated model and having to change direction constantly.

Is there a was I can solve this problem with a setting?

Or is it just how the program works? converting to a pixelated model? Would Rhinocam or fustion 360 work the same way?

Hope this makes sense!

Thank

Nick

Part of the problem and maybe the solution lies in your motion control software. There is usually a "CV" (constant velocity) setting. If this is turned off, the machine will stop at every change of direction and then restart. With it on, the machine tries to keep up a steady cutting speed by very slightly (and generally imperceptibly) rounding off the "corners" but giving a much smoother motion. Much smoother! Anyone who has been through this will know what I mean! This explains why straight cutting is fine but highly-faceted cuts are not.

This also helps the quality of finish doing the kinds of thing you are doing. I've just finished a project which involved copying a 3D relief carving by measuring the original across a 1mm grid and converting the mesh into a highly-faceted model and hence toolpath. However, using the appropriate CV setting I have a very smooth finished result. I also used vCarve for generating the toolpath although my mesh model came from other software. However, I would expect F360 or any other CAM software to do the same thing - it's generating a toolpath to match the model and the answer is at the motion control level.

Good luck!

Thanks for your response Neale.

Is the constant velocity setting something I should be able to set using the CNC control panel? The CNC I am using is a AXYZ 4008.

I will also contact AXYZ and see if they can advice.

Cheers

I will come straight out and admit that I greatly prefer Rhinocam to Vcarve.It ought to be better,considering how much more it costs and it has the huge advantage of working with the file in it's native format.Which avoids having to export to an inherently faceted format.For your current setup,can you adjust the element size of the .stl mesh in Rhino?It will increase the size of the file a fair bit and give you a leg up when importing an already finer file .

Can't say anything about RhinoCAM - I have used an older version of Rhino itself (v4, I think) and concluded that as an engineering CAD application it didn't suit me - but I'm sure that things have moved on a lot since then. However, my copy of Vcarve produced a gcode file - and this was just for finishing, not roughing - of just under 50000 G1 straight-line moves in 3D and the finished item shows no sign of facets, so while it might not be perfect, it is perfectly capable of doing the job. My starting point was a rectangular grid approx 150x120mm with heights at 1 mm intervals, so the actual mesh model was relatively coarse, and the CV function in the motion controller smoothed it all out and there was no jerkiness or other roughness in the cutting process. So I don't that think that the way Nickn has produced his gcode is, in itself, flawed even though there might be better methods of generating the model. I guess it comes down to whether you want to do the smoothing as part of the model generation or while processing the gcode. I have no view there except that I've found a way that works for me!

As for where to find the setting - I could tell you how using Mach3 or myCNC (the two motion control applications I use) and I'm sure it would be easy to find for UCCNC. but I have no idea what AXYZ use or what their control panel looks like. But a controller that does not have this option sounds unlikely, so it must be there somewhere!

I have been and am a user of Vcarve and Aspire and I think you will find the stl model has not been created fine or good enough to produce an acceptable finished product,
I am designing and cutting in 2 1/2d and 3D and find some imported stl's are not up to fine detail,

Phill

Ok, I reckon we have two issues here.

First - the original question - is the jerky motion. I would be 95% certain that this is down to the CV setting. Get this right and a lot of what you are seeing will disappear. My guess is that your CAM application is generating G1 straight-line moves following the facet faces and the machine does a start-stop at each corner. If most of your work to date has been straight lines and circular arcs/curves that can use G2/G3 circular arcs motion would have been much smoother.

Second - can you improve the situation with a better, finer-mesh, model? The answer to that one, I suspect, is that it all depends. My last project was a shallow relief carving over a 150x120mm area, but the Z only varied by about 6mm over that area, with a lot of smooth surfaces. So, my relatively coarse mesh gave good results. A deeper carving with a lot of up-and-down in it might not have worked so well. In either case, though, both the CAM systems I use (vCarve and F360) would generate G1 straight line moves, and maybe a finer mesh would have generated even more corners. In any case, the effect would be masked by the use of CV. But then the end result will change depending on the tool used (esp. diameter), stepover, etc. I'm not sure if there are any CAM systems that are clever enough to generate gcode arcs for this kind of thing. I did once do some 3D carving like this where, seen from close up and in the right light, you could just make out the facets. Clearly the model mesh was a bit too coarse. But given that it was a house nameplate that would only be seen from at least 3-4ft, it was fit for purpose. It all depends...

thanks for the replies.

I'm looking into the CV setting. curves cut fast from a 2D drawing using Artcam, it just 3D Vcarve models that have the issue. I have sent an email to axyz to see what they say. I don't use motion control software on the pc, I'm assuming this software is on the CNC itself? and controlled using the control pad? I just save the toolpaths in Vcarve then drop them into a folder on the cnc linked by Ethernet then open using the control pad. sorry for my lack of knowledge, The company I work for manly cut 2D stuff but recently we have been getting lots more 3D work. The CNC technician left so I have stepped in.

Is .stl the best format to save the file in? they are mostly 3dm Rhino files originally. I save the .stl file with high ish detail about 0.0001 setting.

I have also contacted Vectrics and sent them the .vrc Vcarve file to see what they say.

cheers

It's pretty likely that your 2D-derived cutting uses straight and circular arc moves, both of which can be handled efficiently by the motion control software. It's non-circular curves, or lots of sharp corners, that give problems.

For most hobby users, the motion control software runs on a PC and in effect takes a gcode toolpath file and via some piece of electronic hardware (as simple as the PC parallel port through to dedicated external hardware modules of more or less sophistication) converts the gcode toolpath into the electrical signals that go to the machine. In your case, the motion control elements are built-in and effectively part of the machine although technically they are still there under the cover somewhere. And it's the parameters associated with that bit of the control system that you probably need to tweak.

Personally, I would think that STL is as good a format for transferring a model into vCarve as anything else - and there aren't a whole lot of other formats that vCarve can use anyway! So the things you can play with are mesh density and any related controls in Rhino that are used to generate the mesh. In my case, the mesh size came from the spacing used to probe the original but if you are generating the mesh within Rhino from a 3D model, then you might have more options. Not something with which I am familiar, I'm afraid.

I don't think Vcarve will import a 3D object in any format other than .stl .Come to that,I don't know enough about Vcarve to know if it has a CV setting,I have worked with a couple of controllers that would accept a G96 command to achieve this kind of outcome but they were a bit more sophisticated than an AXYZ contrroller.There may be things you can adjust within the parameters of the controller to improve things.Do you have any idea what the optimal acceleration settings for the machine might be?There may be,indeed should be,a manual for the machine that includes such details and the original settings may have been tweaked by the departed tech to speed up cycle times.It could be useful to compare what the current setting is to the factory figure.