machine settings

I am running the first tests of the 5th axis setup and it seems madcam is not honoring the maximum tilt angles in the settings screen . I am currently get tilt angles above 200 degrees

any ideas ?

The max and min angles that you set for the machine is used for preventing any axis to exceed the angle limits, but only if there is another solution.
There are always two solutions depending on the 4th and 5th axis. For example: A30 and C120 is equal to A-30 and C300 or C-60. madCAM tries to find the shortest way to another solution if A or C exceeds any of the axis limits.
If there isn't any solution, it will not work anyway and you will have to recalculate the toolpath with another drive surface or by setting limits to the machine head from a vector. It is possible to set angle limits of the machine head, measured from a vector. If the head tilts more than the limit, controlled by the drive surface, the head will be locked to the angle limit. (See screen shot below)

Attachment 448482

/Joakim

thanks for answering , for some reason madcam is still not honoring the limits set for the machine -10 and 100 degrees in both machine setting and drive surface settings even with simple flat drive surfaces tilted . I am stumped as to what to do to fix this , any other ideas other than the above responce which we were already doing ?

I will email you the model as it seems I can not upload 3dm files here

With these kind of drive surfaces, there is no need for angle limits set with the drive surface. In this case, it seems to be a tolerance problem related to the given angle limits of the machine.

Drive surface 1 generates angles for indexing A=+95 and C=-10 and that works weell since the angles are within the given machine angle limits.

Drives surface 2 generates angles for indexing A=+100 and C=+10.579. Since the machine angle limits of the A-axis is set from -10 to 100, the A-axis max limit is exceeded and madCAM tries to find another solution by rotating the C-axis 180 degrees. The angles will then be A=-100 and C=-169.421 and that will not help, since the angle limit of the A-axis is still exceeded. There is no solution for milling this with the given machine angle limits.

For solving the problem, you can set the machine angle limits of the A-axis from -10 to 101 degrees. Then it will be a tolerance that will work in this case.

It would also be possible to set an angle limit with the drive surface from 0 to 99.

I hope this will give you some help.

Regards,

Joakim

thank for getting back to me so quickly , I get what you are saying but i am not quite sure why Madcam using a drive surface facing the same way on the same part tries to do the complete opposite ??

One thing I tried after sending you the email was using the same drive surface but flipping it in place 180 degrees so the back side was facing the part then it worked fine , even though I tried flipping back and forth the surface direction arrows in Rhino with no effect . Why would flipping the drive surface create the correct output?


best regards
gregore

- - - Updated - - -

PS I am still using windows 7 if that makes any difference

thanks

It's just because the drive surface generates an angle of the A-axis that is very close to the physical angle limit of your machine.
The A-axis and C-axis are rotated to a position where the cutter is perpendicular to the drive surface. Drive surface 2 generates an angle of the A-axis that is very close to 100 degrees, too close to your angle limit of your machine.

If the drive surface normal vectors generates an angle for the A-axis that is slightly above your maximum machine angle limit, there is no solution for your machine in this case. By flipping the drive surface in this case, will generate an A-angle that is lightly below your maximum angle limit for your machine and then it works.

Another way to solve the problem is to rotate your part 1 degree around X in Rhino before creating toolpaths.

Regards,

Joakim

I have continued to play with the same model changing the angle of the drive surfaces to be below machine settings , cutting waxes to test out different cutting strategies

but i have noticed an issue that I have never had to deal with with 4 axis , on the same model i sent you: when it changes from cutting one pocket to the other #2 to # 3 Z does not retract enough and when A tilts back up the cutter tip catches on the inside or catches on the way back down to start the new pocket cut , is there some way to control retracts between tool paths in madcam or is this done in the post ?


thanks
gregore

I think the easiest way is to use the toolpath change section in the post processor. This section in the post processor will take action when moving from one toolpath group to another, even if the same tool is used. Below is an example of how the toolpath change section can be used.

*TOOLPATH_CHANGE*
G0 "zhome" (Go to the top off the madCAM box)
G0 "azero" (zero the A-axis)
*END_SECTION*

This will move the cutter to the top of the madCAM box and zero the A-axis before continue and move to the next toolpath.

Regards,

Joakim