[inflateable]

Hi All,

I hate writing post processors, everytime you think you've finished something else comes up...

I'm having trouble getting my lathe post to not resolve rapid moves.
Basically, my operators don't like diagonal rapids, because they can't easily tell where they are going to end. They prefer I move in Z first, then down in X.

No problem.

Edgecam is showing me on screen a 'safe approach' moves, doing exactly that - moving in Z first and then down in X, but my post insists on throwing out resolved rapids.

So I want, and I see on screen:
N10 Z10.0
N20 X0.0

But I get from the post.
N10 Z10.0 X0.0

In the 'machine parameters' part of the code generator there is a check box 'resolve rapids' which is supposed to do exactly what I want, but it has no effect. So something somewhere else is overriding that option I'm guessing, but I can't find it.

Anyone?

[cam1]

Try this (just to troubleshoot)
When you uncheck the resolve rapids box and Post do you get the same code?
If yes, then have a look at the setup for that tool. There may be an option there to control the movement. Don't forget that sometimes "job setup functions" onlt take effect the next new program.
I'm a Mastercam lathe guy, but I've got alot of experience with de-bugging. I don't really care what application it's for. Code is code....

I can totally appreciate your frustration. I've had to build my own post for Solidcam, and re-work the one for my lathe....I just wanna make this simple stinking part, without having to modify the post (sound familiar)

regards

[inflateable]

Yeah, exactly the same code whether 'resolve rapids' is ticked or not.

Like you I suspect a setting in the tool somewhere, but I can't find anything that would have that effect.

I'll try creating a post from scratch from the edgecam original config files and see what that does - if it still doesn't resolve, then I think I found (another) bug.

Thanks for the help!

Jon

[chrisryn]

try unchecking 3d rapids in code wizard

[inflateable]

ah, the box underneath 'resolve rapids' you mean?

Greyed out, presumably because this is a 2 axis lathe post.

[chrisryn]

You have to change it in your code constructors example:
Rapid move:
[DELETE][BLKNUM][RAPIDGCODE][ZMOVE]
[XMOVE]
Rapid After tool Change:
[DELETE][BLKNUM][<C>RAPIDGCODE][XMOVE]
[ZMOVE][COOLANT][SPEED]

This will output like this
G97 S2500 M3
M8
G00 X2.5725
Z0.0421
G71 U0.1
G71 P10 Q20 U.02 W0 F0.01
N10 G00
X1.6
G01 Z0.0
G01 Z-1.4687
G01 X1.9125 Z-1.4688
G03 X2.2023 Z-1.609 R0.145
N20 G01 Z-1.6937
G00 Z0.0331
X1.7299 G70 P30 Q40
N30 G00
X1.6
G01 Z0.0 S2000
N40 G01 X0.0
G00X4.0
Z6.0
M9

[Mike Mattera]

I know that for "Rapid To Toolchange" this is the standard code...
[DELETE][BLKNUM][CANCELTLO]
[DELETE][BLKNUM] G28[U0][W0][SPINSTOP][COOLANT OFF]
[SECOND_LEG]

"Second Leg" sends it to "Rapid to Toolchgange 2" which, if your resolved rapids are set right will make the 2nd axis move (i.e. in your toolchange you specify Move X first, Z will be in the second leg to the toolchange move).
I dont know if you can force it to make X first or Z first moves when approaching the part. In all of the PCI's that Steve Harrison has written, he forces a Rapid to a Z and then Rapid to an X for his pre-position of the cut.

I think that may be the only solution. Do a Rapid to the X, Then Rapid to the Z (or which ever order you want it output).


Mike Mattera
Tips For Mfg

[inflateable]

...yes, that's what i'm doing at the moment, using a rapid line in edgecam.

I'm a little bit wary of changing the post to force an X first then a Z (or vice versa) as what I see in edgecam might not be then what the post throws out, which is asking for trouble!

I've got a pathtrace bod coming in the next few weeks, so I'll find out then!

Thanks for all the replies, this forum is a saviour!

J

[felixandrea]

It sounds like you’ve tried a lot! If you’re still worried about editing the post and it not matching what you see in Edgecam, waiting for the Pathtrace experts to come is probably the safest option. Post editing can sometimes cause some nasty bugs, especially if the animations aren’t showing up correctly. Hopefully they can sort it out for you!
rice purity