Unwind without retract?

[bmilford]

I am cutting a foam pattern with a Thermwood 5 axis machine and when I posted this code it initiated a unwind without retracting the tool. 

The toolpath I used is Curve 5 Axis, it is a custom cutter that just has to follow a line to cut a profile into the part.

G00 X14.3867 Y31.0298 C180. B-45.7304

.
.
.
.
G01 X7.8847 Z-5.6122 B45.7308
G01 X7.1686 Z-4.9141 F2100.
G01 X2.1562 Z-0.0279
G01 X2.1578 Y27.895 Z-0.0263 C0. B-45.7247 F6500.
G01 X7.1697 Z-4.913 F2100.
G01 X7.8857 Z-5.6112 F25.

Luckily it is just foam, but i can live without the crescent shaped gouge in the pattern.

Normally i would see a unwind / retract move in the code.

It is posting out with the Post I got from Thermwood, it doesn't show in verify or backplot in Mastercam.

Does anyone have an idea how I can avoid this? I don't know why it would need to unwind to return to the starting position of B-45.7304.

I have added to the Retract distance to hopefully avoid the gouge.

 

Thanks,

Brian

[MATT Q]

How are you driving the curve 5 path (surfaces, lines, etc...)?

[crazy^millman]

You need to prewind the head and do your best to make the toolpath stays within the C travel limits. I would sometimes split a solid in half or move the solid so the split line was where the travel would never want to go more than 380 degrees in one move. Don't do anytime of motion where the head needed to keep going machine is not capable of that movement. I also make my own retract moves where I control the head all the way from start to finish in a cut. Last thing I want is some stupid post that has not idea what I trying to do start doing unwinds and scrapping a part. Always know what your machine is doing when programming Mastercam. Anytime a programmer programs without knowing what will run on their machine they are asking for trouble. 

Here is link to the samples I posted up over the years on how to do this. 

Unwind Example #1

Unwind Example #2

Unwind Example #3

[bmilford]

I projected a curve onto a surface and used the surface for the tool axis control and followed the curve.

The curve is basically three arcs, one on each end 1" radius 45 degree of arc length, and the middle is a large radius arc (almost flat).

I guess I didn't show enough code to show the tool entered the cut a C180 B-45ish, rotated only B as it cut across the part to C180 B+45ish. It then retracted (not high enough) and stepped over to the next line. Before it fed into the cut it reversed B and C, with out the unwind/retract the post would normally call for when reversing B and C. 

What I am trying to figure out is why didn't the tool just run back from C180 B+45 to C180 B-45? 

I browsed through the code before I ran it and was distracted by a line "(p_reverse_incut ------------)" in the code. I missed the C flip. 

I got done cutting the part now I'm just trying to learn how not to do it again.

Thanks for the help!

Brian