sheetcam.com

Hi, this is not a specific SheetCam question, but I hope someone can point me in the right direction.
Having been formally trained on the lathe and mill, I would like to make a finishing pass when cutting the external contour of a piece.
That means that there would be a normal contour operation with a slight offset of probably 0.05 to 0.1 mm, followed by a tool-down path that would take about half the offset and a final high-speed pass in reverse-cut that would take the rest of the offset.
I believe I understand enough G-code to produce the relevant code, but it would be tedious and above all, subject to possible errors.
Anybody have advice, comments?

You can do this when you specify your operations. First roughing pass leave your stock as an offset. Then write another operation right after it with no offset. I do all my passes climb cutting, not sure why you would ever want to run a reverse direction pass, but if you do, you would just have to change the climb cut option box in the operations parameters.

Well, that's more or less what I thought first; however, as I said, it's error-prone.
That would mean first offsetting the contour operation. I would need to enter a tool diameter larger than the actual by let's say 0.1mm, which is the first source of potential error, unless there is a command that does it...?
Then I would have to make another contour operation with a slightly smaller offset, e.g. 0.05mm and a single pass with the tool down. Second source of potential error.
Finally there would be another tool-down contour without offset but reverse-cut.
Reverse-cut is a well-known technique for finishing - at least it was when I learnt milling. The chip is lifted intead of pushed in.
I wonder why this is not implemented since other similar finishing operations exist in drilling and pocketing operations, but only relevant to the Z-axis.

This is what finish allowance is for. Set up your roughing operation with a finish allowance of say 0.1mm. Next set up your finish operation with no finish allowance. This isn't combined in one 'roughing with finish' operation because you could be using completely different settings for your roughing and finish passes. For instance you could rough with a rougher mill with multiple Z passes while finishing with a different cutter in one pass.

By the way you can enter negative values in finish allowance, taking off more than the drawing specifies. This makes it useful for fine tuning precision fits etc.

With CNC machining the general practise is to always climb cut as this usually gives a better finish and tool life. Most CNCs have very low backlash so they don't grab when climb cutting. It's also better to avoid really shallow cuts (e.g 0.05mm) as this accelerates tool wear.

What Les said... plus you don't change diameter of the tools, you just change the finish allowance offset. I've been running CNC mills and lathes since the 70's and never run a conventional pass for finishing and always have my finishing pass taking at least .005" or .1mm or you are rubbing and not cutting.

Thanks for your answers. I understand I'll have to create an additional G-code for finishing.
Your comments made me realize that the finishing pass I had learned in the 60's was done with a straight-cut bit. The only straight-cut bits I see for CNC are one-flute. I really have to forget some of the things I took for granted.
EDIT: I can find 2-flute straight-cut bits, but they seem to be restricted to wood and plastic, not AL.