Setting up VM5

[dneisler]

I just bought a used CNC mill, and it has VM5 with it. I am lost.
I have drawn a simple 1" x 1" square that I was trying to have a pen draw on this mill to test how it is working. I cannot figure out how.

I select the region PolyLine0.
Choose 2 1/2D profiling.
Generate


What post processor do I use for HobbyCNC Board?


This is what I got for a 1 x 1 square profile cut.
G90
G20
S4583M3
G0X-0.5Y-0.25
Z0.3125
G1Z0.F7.3
X-0.25F3.7
X-0.2012Y-0.2452F2.7
X-0.1543Y-0.231
X-0.1111Y-0.2079
X-0.0732Y-0.1768
X-0.0421Y-0.1389
X-0.019Y-0.0957
X-0.0048Y-0.0488
X0.Y0.
Y1.F3.7
X1.
Y0.
X0.
X-0.0488Y-0.0048F2.7
X-0.0957Y-0.019
X-0.1389Y-0.0421
X-0.1768Y-0.0732
X-0.2079Y-0.1111
X-0.231Y-0.1543
X-0.2452Y-0.2012
X-0.25Y-0.25
Y-0.5F0.393701
G0Z0.3125
M02

[chmillman]

Several things going on here.

First, I assume your controller can handle arc moves (G2/G3).
The four lines of your code here
Y1.F3.7
X1.
Y0.
X0.
are the actual square, the rest appear to be the approaches. Looks like you have 1/4" arcs set plus an additional 1/4" straight section. By default, VM does not have circular arcs turned on. So all that is divided up into straight segments. First, go into preferences, machining preferences. Make sure all three top checkboxes are cleared.

Check your operation entry/exit tab to change the approach parameters if desired.

For other similar operations, it may also be helpful to go to the last tab in parameters (Advanced Cut Parameters), check the box "cut arc fitting" XY plane and put in a tolerance about the same as your main operation tolerance, which will try to fit a maximum of arcs to your linear moves if possible. Works OK, but it's not perfect. --ch

[rklosinski]

I was reading this post, and you just happened to answer a question I had regarding the generation of arcs. I followed your instructions and unchecked the boxes.

What I got was arcs... in vengence! Instead of generating three small pockets, I got three large pockets. I've been trying to use visual mill, but might switch to sheetcam, as it generates IJ arcs and does a better job on pockets.

Rich

[DareBee]

VM will generate IJ arcs, sounds to me like you need to configure the post processor to make the output you desire.

[vertcnc]

I have a similar problem. I have a coned shaped object created in solid works. When I create the tools paths in VM 5 all the curves are short line segments. I do have all three check boxes in the machine perferences unchecked. I totally stumped. I am using the post proccessor for Mach 3. Could it be the way the file is saved in solid works and then opened in VM? Any help would be appreciated. I could post the file if needed.

Thanks

Tim

[chmillman]

In some 2D ops like pocketing, there is a cut arc fitting checkbox on the advanced parameters tab. This will force the output to be arcs if the parameters are set correctly.

In principle, for 3D ops, the output will always be line segments, if you want to convert to arcs you need to do the arc fitting in the toolpath editor for each toolpath you generate. Double cick on the toolpath icon in the browser, that opens the editor, there is a button for convert to arcs. There is a dialog with settings.

In actual practice, for 3D ops, I found it very hard to set VM's arc fitting up so that it actually works, so I never bother. Part of this may be due to the fact that a number of VM's 3D routines don't really produce toolpaths smooth enough to be arc fit in one plane, no matter how you set the operation up. Or maybe their arc fitting routines are just poor.

My machine doesn't really need arc fit for 3D stuff, having a high speed control capable of processing large amounts line data quickly. The files are big, but so what... --ch

[vertcnc]

Thanks for the suggestions. I agree that the short line segments most times are not a problem. With Mach 3 control it is a little slow processing all these lines. With this particular file I can't get the feedrate much above 20ipm and have smooth motion. It is a radial 3d tool path that cuts a taper around a 2 1/2" radius about 3/4" tall. I was just trying to speed up the 4 hour job. I will try some of your sugestions.

Thanks again
Tim