[stevespo]

I am doing some simple 3d milling - guitar fingerboards with different radii (like a section of a cylinder). Easy enough to create the radiused board and generate a toolpath. But...

How do I control the "smoothness" of the machined 3d surface?

Like many things in BobCAD, this really has me baffled. The gcode consists of many straight line moves, not arcs like I would expect. The number and length of these lines determines how smooth the machined surface is. I do not know what setting to change to change this.

At one point each arc was made of 7 moves - very coarse. Tech support had me change some settings and the arcs were then made by performing 50 moves - very smooth. After trying to solve some other problems, the support person made some changes, and now my arcs are 25 moves.

This is probably adequate - but I just want to know what exact setting determines this. Arc Interpolation error is a logical candidate, but doesn't seem to do anything. General Accuracy didn't seem to help. Set Path -> max error for arcs? Again, didn't seem to help.

Thanks,

Steve

[Jim Estes]

Stevespo,

Most of the time any 3-D machining toolpath will be a collection of line segments, very few machines will actually cut 3D radii.

When you generate the toolpath, you can set the control parameters in the window right below where you set the step over amount. Also, with compoiund radii, you will want to cut in the direction of the largest radius, this will help to create longer line segments. For instance, in your case, the fingerboard will have a smaller radius across it (side to side) and a larger radius lengthwise (length of the board if at all radiused). Setting the tolerance very low will help, but what really helps is cutting in the direction of the longest radius. This is controlled by the toolpath angle that you set.

If your fingerboard is actually straight in the length direction, with a decreasing radii, your toolpath will actually be continuous lines from top to bottom of the fingerboard.

I cut a lot of contoured parting lines, and my machines communication is limited to 9600 bps, so I also get an added benefit from the longer line segments, my machining time is dramatically decreased.

I attached a file, it is exagerated I know.

[The One]

Which Toolpath method are you using?

If it is the 3D Skin function then when you are setting path it depends on the direction of the Toolpath. If it is perpendicular to the Path then the Step Over distance will be the determining factor. If you are runing parallel to the Path then the determining factor is the Minimum Line Length when you are setting the Path.

If you are using one of the Solid Toolpath options then you will want to check the Minimum Line length in the Parameters dialog.

The Arc Interpolation error is used when you are creating code for a 3D arc in the CAD window. It determines the Line length.

Regards

[tjones]

The version 2007 has a new mode of cut called equildistance. This new cut style can give more evenly spaced smoothness on steeper vertical cuts and varying surfness angles/radii.

[stevespo]

You guys are great. That was very helpful information and advice. Jim, my fingerboards are actually simpler than your example, but eventually I will be creating that type of board. You created a nice compound radii fingerboard, right now I'm just doing a single radius board.

I am using the Planar toolpath option from the Solids menu. My stepover is .1", toolpath angle 0, tolerance .0001", and min line length also .0001".

I'm machining the board across it's width - across the narrowest part - parallel to the toolpath. I can see the advantages of going up/down the length with a ballnose bit and a tight stepover. I will try that. I actually ran quite a few tests and my best results (fastest, least sanding) came with a 3/4" straight bit and working side to side, up and down that little hill of an arc. I'm sure it's worth more experimentation.

I will play around with minimum line length. These may be unrelated, but my general accuracy is currently .00001" and my chain gap is .0001". I believe these were set by tech support while troubleshooting another problem with "crop circles" - and I have some ideas for solving that as well.

Thanks,

Steve

[stevespo]

I'm definitely getting different results by changing min line length - but it's not clear how it's really working. A super small value (min val) of .0001" seems to generate fewer movements than a larger value like .001". The best resolution seems to be coming from .0007" - so I will stick with that. I would assume the smaller the line length, the higher the resolution, but maybe that's not really the case?

Steve

[Jim Estes]

I get crop circles sometimes even when trying to do 2-D milling, the cause of my circles was having large radii in the contour instead of line segments. There is a conflict when having these large radii with the I and J value being close to X0.0000 and Y0.0000. The best I could tell is that I would get errors because of this, so to solve the problem I offset the Origin to a point far from the center of the part, this solved the problem very well.

Jim

[tjones]

This type of error can actually be caused by a couple things that can easily be set in your NC CAM. First try outputing circles in no more than 180 degree sections. Then try outputing either I J or then radius type of output to see if they act different. Also try incremental then absolute output to see if that makes a difference. Also don't output equal values of x,y coordinates.

[Jim Estes]

My machine doesn't accept the R value when doing G02/G03, and I am not sure that it would accept the absolute values. I figured out that just offsetting the origin and the fixture offset on my mill and it doesn't give me the circles.

Also, I am usually pretty compulsive about verifying the programs before I run them, but I have had to use the metal adding machine several times because of the simplest of tasks would end up doing a lot of damage to my parts.

Jim

[The One]

You can also correct the problem on the geometry level without and Offset. The reason you run into these arc segments that create a full circle is commonly related to non-tangent arcs. BobCAD is setup to create an arc around a corner, even if the resulting arc is too small for the machine care about.

Try this next time:
Select your chains.
Click on Change => Reorganize => Make Arcs Tangential.
Set the Minimum Accetpable angle to .001 and the Max. Angle for correction to something like 10-20.
Then Click OK.

This should reduce the occurence of the so called "crop circles".

Regards