|Home » Forums » CNC » Message||Login|
You are not logged in. Consider these WOODWEB Member advantages:
AlphaCam and open contours10/7
I'm new to using AlphaCam (2013 R1 SP2) and learning as I go...when cutting open contours I can't seem to get cutter comp to post out. I needed to cut several large radii (200" and bigger) for curved wall caps.
I have done to following:
All three give me the same code for cutter comp, in this case C=0 (which is no comp. for the SCM router).
I tried lead-ins as a sloping line, line with arc, arc only, the above lead-ins with an angle added (5deg.).
All post out the same comp code (C=0).
So what is the trick to getting open contours programmed with cutter comp and posted out?
Any help would be appreciated.
Tool Center just means no code for cutter comp. tool path data in generated by the radius gotten from the tool you created. C0 or G40 on most machines. by default there is no cutter comp, so no code needed.
G41/42 Tool Center. Same as above, but the post outputs a G42/C1 for RH comp or a G41\C2 for Left hand comp. With this style of comp, a new bit should have a 0 value in the radius for the tool at the machine. A sharpened bit will have a negative value in the registry at the machine. This is hard for a lot of people to understand, but the machine is only compensating for the difference between a new and serviced tool. (Best way to go with Fanuc and other similar controllers.)
G41/42 Machine comp outputs the code so that in order for the part to be correct, the machine compensates for the entire radius of the tool. In this scenario, you need to put in the correct radius at the machine, or diameter. Many years ago Xilog required diameter, not radius in the tool file. This style should also produce a G42/C1 or a G41/C2.
In many controls, the comp is turned on and off by a G1 line with a movement = or greater than the value being compensated. Don't think SCM's version requires that. Maybe checking apply compensation on Rapid will turn it on. Good luck. Hope that helped.
Have selected Apply Compensation on rapid approach/retract?
Have you tried breaking the arc into two pieces?
Thanks Mike and Rob,
Our Xilog tool file asks for tool diameter. I have been using G41/42 Machine comp with the actual diameter entered into the tool def file. I also have checked the Apply Compensation on rapid approach/retract box
So I'm at a loss as to what to do to get comp to work for the open contours.
That doesn't make sense that you get right hand comp output on closed contours but not open. When you turn on ghost tools, it shows that the tool direction is set to right side? View-Display Options-Ghost Tools.
So have you tried breaking the entity into two pieces and then posting?
Iv'e tried it several ways and it works every time.
Thanks for the responses. I haven't gotten a chance to revisit this issue. I've been making parts. All closed contours fortunately. I'll be able to take another look at this on Monday. Thanks again.
Have you checked, "Apply Compensation on rapid approach/retract"?
Thanks for all the responses. I have it working for me now. I'm not sure what I was doing wrong but it seems that when choosing the tool direction on the open contour, if "Set Start Point on Closed Geometries" is set to anything other than "NO" when picking the contour, the process doesn't work properly. So I now make sure that "NO" is set for this choice.
I never would have thought that being your problem. My normal choice for open geometry is to choose reverse direction then right or left side. That is the quickest way to get what you are after if you aren't aware of the direction of the geometry. Worst case scenario is that you have to click on it twice and you are ready to go.