Printable View
Thanks for any help in advance.
Is there any way to use tool compensation in the Winmax controller (VM20) after we upload a program? We have tried several different ways and so far no luck. In other words we want to adjust for tool wear without going back to the CAM program
Dennis
Winmax handles cutter comp just like any other gcode control. You need to turn on cutter comp in featurecam (post options) and make sure it's enabled in your post (It is if you're using the stock winmax post that comes with featurecam). If you turn it on and find G40, G41 and G42 here and there in your code then it's working.
HOWEVER;
I'm not a huge believer of using cutter comp with cam systems (I use featurecam, have hurcos and other machines), since there is a possibility of moves happening that don't show up in the simulation. I have been bitten with this in the past with threadmilling, looked good in the simulation, but the machine interpreted it differently because the comp on move was so small, starting going the wrong way, scrapped an expensive part and an expensive threadmill...
It's the same reason I avoid using canned cycles in cam programs. Output simple straight gcode and what-you-see-is-what-you-get. Start messing with comp and cycles and you might get the odd nasty surprise.
It's worth noting that featurecam's simulation is NOT a real backplot of the code and the accuracy of the simulation relies HEAVILY on the quality of your post.
Long story short, if you do a lot of single parts without dry runs, leave it the way it is!
There should be a comp selection in your CAM software, Wear Closer/Wear Away or something along those lines that enables machine comp & posts the G41/G42/G43 code.
On the Hurco control, you have one screen for tool height comp and one screen for tool DIAMETER comp. The diameter comp is the second screen on mine and you have to look to make sure you're on the dia. screen as they are both identical save for the one word. There are comp registers #'s 1-200 on each screen. Normally you pick a comp register to match the tool number to keep things simple. Run your part, measure it, enter the amount of comp. you need to correct the size. No need to alter your program.
If you are comp'ing a round bore/boss (closed pocket etc), the amount of comp entered on the control is the amount the diameter of that bore/boss will increase/decrease. If you are comping a profile, the amount that you comp left or right of the tool path will be half of the comp value entered on the control.
You can use positive and negative values as well. If you're trying to sneak up on a slip fit bore, you could start with a negative comp value (assuming you're climb milling and comping right), check dims, and keep increasing the comp value on the control in the positive direction & re-runing the finish pass until you reach the fit you're after. (Hope I've got my directions right)
It's really easier than it sounds but be sure you've got the right number of decimal places before you hit the BGB. Look away, look at the part, look at the control again.
There is a softkey to clear all comp values, it's a good idea to do that when you're done with a part program unless you will use that same tool in the next program.