1. ## Accuracy

What I must do to improve the accuracy of toolpath in Sheetcam. A dxf file with nominal dimensions are cut bigger with 0.2 mm if I setup the dimension at Nominal -0.2 it is smaller with -0.3-0.5, if I set dimension at Nominal +0.1 it is bigger with +0.35+0.4 and so on. Never I get the same difference...Could somebody give me a clue. Also, I would like to ask what strategy to apply when I cut circle inside. The circle is perfect except the fact that at the point where the endmill is starting the cut oversteps the rim of the circle, with let say 10% and the rim has a small print. So, the hole is not absolutely round it has a small round chanell along of it (on vertical axis at the place of starting - hope, I could explain in English).

Thank you,

Zoltan

2. 1) Are you changing the dims. with -0.2 pr side (or radius)? If so, then it will give the double difference. the same is the case for your positive adjustment. Or are you talking about it radius compensation? Then you must put in the radius and not the diameter of your tool.

2) To get the a nice round hole, you need to enter your circle path, while using a circle. See following simple example"
G00 X0 Y0;
G00 Z?
I-0.5 (CUT HOLE DIAMETER = 1.0"
X0 R0.25 (MOVE BACK TO CENTER OF HOLE)
G00 Z1.0
THAT IS HOW I DO IT ON SIMPLE SMALL HOLES WITH NO RADIUS COMP. YOU CAN CHOOSE TO ADD RADIUS COMPENSATION ABOVE THE HOLE, IF YOU HAVE NO SPACE IN THE HOLE (BUT BE CAREFUL!!!!!!)

OTHER IDEAS FOR THIS GUY ARE WELCOME. MY WAY IS NOT THE ONLY ONE.

E.T.

3. SheetCam's maths is usually better than 0.01mm. It sounds like you are having problems with tool flex or machine flex. Define your tool the correct size and use a finish allowance of 0. Cut a circle and check the dimensions. Now reverse the cut direction (in the cut path tab, select climb cut). Cut the circle again. If it comes out a different size your machine or tool is bending as it cuts. All machines do this to a certain extent. It can be difficult to compensate for this. One method is to cut the part slightly oversize then take another very shallow cut to get it to size. As the shallow cut does not stress the machine you get a more accurate result. Here is how you would go about doing this.

Define your cut process as normal but set the finish allowance to something like 0.1mm. This will leave 0.1mm for the next cut pass. Now define a new cut process with a finish allowance of 0. To reduce the mark left when the cutter plunges into the work go to the cut start tab and select arc leadin and leadout. Set the leadin/out size to something like 2mm. Using climb cutting can improve the finish.

You can adjust the finish allowance to adjust out any remaining flex but remember that the amount of flex depends on the cut depth so you may have to cut a few trial parts if you need high accuracy.

Les

4. OK. Thank you. This is very helpful. I did not know these things. I will try it. I do not think that the fenomen I tried to explain is related with the machine. I will explain why. If I cut the same dxf from diferent pieces of material I get the same size of hole. The same result I get if I have multiple holes on the same part, no matter their position. My problem is the discrepancy between the solid model which I save on dxf format and the cut result. It keeps the same dimension for all holes but I have no correlation between the value setup in cad drawing and cut result and I can not see how to get in real what I draw. It means that never know what would be the size of holes if let say I have then holes same diameter, but they will be eaul each other.

Thank you,

Zoltan

5. Sorry. Typing errors.

....ten holes same diameter....
..they will be equal each other.

6. Hi Zoltan,

Can you please do the following: load one of your drawings, create the cut processes then run the post processor. Save the job then go to Help->Create a support file. Send the support file to me les_@_sheetcam.com (remove the underscores). I will then be able to copy your setup exactly and find out if it is a drawing or code problem.

Les