|Home » Forums » CNC » Message||Login|
You are not logged in. Consider these WOODWEB Member advantages:
New CNC offsetting approaching 90 degree corners6/3
When cutting profile cuts at higher speed, my router shifts laterally as it approaches a 90 degree corner. It gets worse the faster the working speed. At 300 ipm, it offsets probably 0.05" about 1.0" from the corner. As I slow the speed, the offset and distance lessen proportionally. I have to slow down to 50 ipm before the finish is tolerable, but I'm not happy with that. Any clue what this might be?
I plan to run a test with different polygons at different speeds and orientations, but so far, I've only noticed this for rectangular shapes.
I used to see something similar on the first CNC we had, where in cutting 90-degree corners at a high feed rate caused a small portion of the cut to be sloped.
What I was told at that time was happening, was that there was a lag between finishing the stroke and beginning the next move. Simply said the cut (movement) in the x-axis begins before the y-axis cut (movement) has finished. Thus the dimple or sloped line at the corner.
You can try a couple things, as you have figured slowing down eliminates the issue. The other is rolling around the corner (cut the corner so that the tool path is a small radius yet the cut is 90-degrees.)
The machine we have now automatically makes these adjustments for 90-degree corners in the control, by slowing as the cutter nears the corner and accelerating as the tool moves away from the corner.
Thanks for the tips. Having to slow down would be a disappointing solution, since it spent extra money to get a faster machine.
I though about how to trick it at the corners to make it stop, like what you mentioned, a loop, a fillet, or something. Just looking at the code, I don't even understand how it "knows" it approaching a corner.
I believe your problem lies within the parameters of the machines control and/or the parameters of the axes drives.
It sounds like a ramping problem. The gantry is moving to fast and not ramping down fast enough. Can you change the ramp speed
I went in and changed the acceleration (increased) of the X and Y axes, and that helped a bit.
I also ended up trying a few other post processors, as the one I was using was generating over 30 lines of code at each corner. I found a couple of PPs that were much shorter and seemed to fix my issue.
Interesting that a PostP would fix it. Our post doesn't show any speed change for corners. The machine control takes care of that. There is a look-ahead- function within the control. When it "sees" a change of direction coming there is an algorithm built into the control that ramps the speed, both up & down. Without that the machine would overshoot the corners. Our machines run on Fanuc controls. The internal program probably has to be different for each machine model. There would be variations based on the moving mass, servo drive capabilities, mechanical stress limitations and how aggressive the router company wants to make claims for it. The changes in speed occur very quickly and are hard to detect visually. Our first router used braking resistors to dissipate the energy generated by the slow downs. Newer controls use other methods. Our first router was "tuned" aggressively and the result when running small parts was a fire in the control cabinet from over heating the braking resistors. The fix was doubling the # of resistors and installing a cooling fan on them. We also put a heat shield between them and the control that had been melted in the original design. Even though the router was out of warranty the company provided the parts and we did the modifications. Some controls have fewer lines of look-ahead and slower processors limiting their ability to respond.
Read the code first and see if there is an offset there. But what you said about slowing down and helping the issue tells me that acc/dec might not be working correctly. The thought of the machine flexing could be possible as well. High speeds are possible 1000ipm+ but a rigid machine. You mention a lot of code to make the corners, what is your CAD/CAM package? Are you generating IJ&K for the corners or using R? What is the brand of your machine? What is the controller, Fanuc, Osai? Need a little more information.