[binfordw]

My table is running good now, but Ive noticed it wasn't quite right in accuracy, I.E, a 3" circle was 2.920", etc.

I have been cutting parts that didnt req specific dimensions up till now so it wasnt a big problem, but I decided to try to get this fixed up today. I drew up a simple test part, and used the steps per inch, motor tuning settings in MAch3 to adjust the finished part size. Is this the correct way to fine tune a table?

I adjusted this till the part matched the CAD dimensions as close as possible, Im not sure if its correct yet but it is alot better than before.

If anyone has any tips or advice on how I can set it up to cut accurate dimensions please let me know,

Thanks

[Kipper]

I treat the cut width as a tool diameter and set the offset in the cad-cam....works fine for me.

[binfordw]

Well Ive tried that with small circles with some luck, but my table is off larger amounts. For instance a decorative part I cut is 25.6" in cad, but ends up 24 1/4" or so when cut. The errors get worse on bigger parts.

[Torchhead]

Set your calibration (steps per unit in MACH) by doing the following.

Replace the torch with a fine point tool. I turned a holder that fits in my torch holder ring. If you can't do that tape a pointer to the end of the torch or on a stable part of the holder.

Start and mark at a zero on one axis. Zero the DRO and use the MDI window to send that axis out as far as you are comfortable on that axis. Example: 42" on a 48" axis.
With a simple tape measure with the dumb end on zero measure out to the pointer and compare that to the commanded distance. Note the error. Estimate it in decimal using your "eye" micrometer.

The see the setting that will get you much closer set up a ratio like this:

Current step setting/X = Actual distance/commanded distance. In the example:

5426.25/X = 41.950/42.000 OR solving for X we get 227902.5 = 41.950X or X= 5432.7175.

BEFORE you reset the steps bring the axis back to zero by typing a "G00 [axis] 0". THEN reset the steps to the new count and sent it out 42.000 again. If there is any error make small fractional step changes until it's dead on. Of you are within .010 in 42 inches you will have an accuracy of .00024 per inch.

Do that with all axis.

Then to get parts dimensionally correct change the tool diameter or kerf offset to get the dimension's perfect.

Once the table is accurate (i.e. you tell it to move 1.000" and it moves that, then do not change the steps per inch (unless you are dealing with a rotary axis but that's ANOTHER story ( ). Use the tooling offsets to get the cut dimensions to be what you want.

Plasma cutting is not that precise. The flame is "floppy" and will bend on curves and can even change width based on the feedrate, cut direction and condition of the consummables. If you can hold +- .025 on a part (assuming your table is accurate to .005 or better per inch) you are doing good.

TOM caudle
www.CandCNC.com

[binfordw]

Got it. Using a marker and travelling 40"+ made it alot easier. I had been changing the motor steps in Mach but apparently I didnt save them correctly, this time I got it and its spot on. Thanks