Linking motion between the tool paths

[Anonymous]

We have a program includes two tool path:

The first tool path is facing with (0,1,0) tool vector; and the second tool path is facing with (0,-1,0) vector. In the *.cut file, the first motion of the second tool path is the (0,1,0) vector. In some moments, this point will cause the problem on the machine. 

How we can move the first point kept the vector of previous tool path?

[TK.421]

If I understand correctly, you are looking to control the orientation of the machine tool between toolpaths?

I will place workplanes where I want to control my machine movement, usually at the start and end points of toolpaths. I then drag and drop these in between toolpaths in the nc program. when the machine tool gets to a workplane, it changes orientation to match the workplane and then moves to the next workplane or toolpath. In the NC Program form, you will need to change 'Connection Moves' to 'Move,Rotate'

If this is what you're looking for, CHECK YOUR CODE to make sure the posted code is doing what it is supposed to!

[Anonymous]

Thank you for the information. 

But I try all the three settings, the *. cut files are identical. 

 

The single tool path has the correct point. But once I put the two tool path in the same NC program, the first motion of the second tool path always keeps the same tool vector as the first tool path. 

[Anonymous]

By the way, my PowerMill version is 2018. I don't know if this setting can have different results because of PowerMill version. 

[TK.421]

the version should not be an issue...

now that I think more about it, I had to have my post modified by Delcam to make use of this. I do remember now! I crashed the machine on a job (small crash, no damage) because Powermill simulated it properly, but that did not carry over to the post. If you are on maintenance, I would suggest opening a ticket for this, and have someone at Autodesk modify your post for this.

I've linked toolpaths the above way for a number of years.  The last year and half, I have my post hard coded to return to azimuth and elevation 0,0 at the end of each toolpath before it moves to the next one. For me, that gets rid of any accident that could happen during toolpath links. Maybe that would be a good solution in your case as well?

[TK.421]

you tried putting the workplane in there with the Z axis in the same orientation as your 'post' Z axis?

[Anonymous]

Thank you very much to share your experience. 

I'm the post-processor builder for the PowerMill program... Because the post-processor reads all the data from *.cut file and creates NC-code. I wonder if it's possible to change the CL file data (cutter location) through PowerMill setting. 

The help shows your idea is correct. But the data in *.cut doesn't change. 

[Anonymous]

I tested that "Connection Moves" in different PowerMill version. 2017 and 2019 both work as expected, but 2018 can't get good data in CL file. 

Thank you for your information. It helps a lot!