Haas question

[Guest]

It's a HAAS, I know

 

Is there a setting to stop a Haas from automatically clamping the rotaries?

 

My post will output clamp/unclamp, it becomes a PITA on a simultaneous cut when the rotary wants to keep clamping/unclamping on it's own

[htm01]

simultaneous on a haas, really jp

I just put a M11 at the start of the cut

[Guest]

I know, I had that coming  

 

I'm not in the other facility but I am told every time the HAAS rotates it locks and unlocks itself

 

so a cut like this

G93 X-.0182 Z.1591 B185.455 F999.99
X-.0124 Z.1609 B190.902 F999.99
X-.0066 Z.1614 B196.35 F999.99
X-.0007 Z.1622 B201.787 F999.99
X.0052 Z.1615 B207.238 F999.99
X.011 Z.1612 B212.69 F999.99
X.0168 Z.1593 B218.169 F999.99
X.0225 Z.1578 B223.613 F999.99
X.0279 Z.1551 B229.107 F999.99
X.0331 Z.1524 B234.558 F999.99
X.038 Z.1489 B240.033 F999.99
X.0425 Z.1451 B245.469 F999.99
X.0466 Z.1409 B250.902 F999.99
X.0502 Z.1363 B256.342 F999.99
X.0535 Z.1314 B261.781 F999.99
X.0563 Z.1262 B267.238 F999.99
X.0526 Z.1238 B270. F999.99
G94 X.0425 F36.

actually plays out on the HAAS like the lock/unlocks are in there.....even though the code doesn't have it...it makes simultaneous essentially impossible 

M11
M13
G93 X-.0182 Z.1591 B185.455 F999.99
M10
M12
M11
M13
X-.0124 Z.1609 B190.902 F999.99
M10
M12
M11
M13
X-.0066 Z.1614 B196.35 F999.99
M10
M12
M11
M13
X-.0007 Z.1622 B201.787 F999.99
M10
M12
M11
M13
X.0052 Z.1615 B207.238 F999.99
M10
M12
M11
M13
X.011 Z.1612 B212.69 F999.99
M10
M12
M11
M13
X.0168 Z.1593 B218.169 F999.99
M10
M12
M11
M13
X.0225 Z.1578 B223.613 F999.99
M10
M12
M11
M13
X.0279 Z.1551 B229.107 F999.99
M10
M12
M11
M13
X.0331 Z.1524 B234.558 F999.99
M10
M12
M11
M13
X.038 Z.1489 B240.033 F999.99
M10
M12
M11
M13
X.0425 Z.1451 B245.469 F999.99
M10
M12
M11
M13
X.0466 Z.1409 B250.902 F999.99
M10
M12
M11
M13
X.0502 Z.1363 B256.342 F999.99
M10
M12
M11
M13
X.0535 Z.1314 B261.781 F999.99
M10
M12
M11
M13
X.0563 Z.1262 B267.238 F999.99
M10
M12
M11
M13
X.0526 Z.1238 B270. F999.99
M10
M12
G94 X.0425 F36.

[Rstewart]

simultaneous on a haas, really jp

I just put a M11 at the start of the cut

 

 

That's what I've done in the past.

[FROZEN]

Just remember if you don't expect a lot form a Haas. You will never be disappointed.

[Eric@HorsepowerInc.]

It's a HAAS, I know

 

Is there a setting to stop a Haas from automatically clamping the rotaries?

 

My post will output clamp/unclamp, it becomes a PITA on a simultaneous cut when the rotary wants to keep clamping/unclamping on it's own

Same here as what HTM01 stated, place a unclamp of both axis before simultaneous action. We do fully 5ax porting here every day, no problems on the Doosan's, but the Haas's seem to clamp/un-clamp. Not as bad as every posted line, but they will do it often and dwell in the port. The solution, make it unclamped until done with that tool path. And yes the Doosan's with 31i a5 and Tsudakomo 5th's blow the Haas's out of the water on speed and quality all day every day.

[Guest]

I far prefer the MAM72 I am programming for but I had to do something for our other shop, plus I am working out a new functioning post processor as they have never had one

 

They've been typing in the positioning for years......no more

[MSL]

Change this Value inside your post.

 

 

 

use_clamp : 1 #Use the automatic clamp Mcode

 

  To

 

use_clamp : 0 #Use the automatic clamp Mcode

[crazy^millman]

Change this Value inside your post.

 

 

 

use_clamp : 1 #Use the automatic clamp Mcode

 

  To

 

use_clamp : 0 #Use the automatic clamp Mcode

 

 

He is not getting output from his post. The HAAS machine on it's own is clamping and unclamping when changing angles and he wants the machine to quit doing that. Not a Mastercam question what so ever.

[Rick46]

Not a Haas guru but sounds like a parameter maybe that needs changed or adjusted in the machine itself ?? JM2C

[Machineguy]

John,

Just for checking, what year is the machine? What software version is in the machine?

I don't have time to check on the my VM3 yet. A little busy right now. I 'll see if it does the same thing.

[GIZMO 21]

 I know this su#@, but I use a manual entry with unlock codes before the 5 axis operation

and a manual operation with the lock codes after the operation, because if you manually

unlock the rotaries you have to manually lock them or else they wont lock.

[djstedman]

 

 I know this su#@, but I use a manual entry with unlock codes before the 5 axis operation

and a manual operation with the lock codes after the operation, because if you manually

unlock the rotaries you have to manually lock them or else they wont lock.

 

This is essentially the same thing I need to do on our Mazak's in order to do simultaneous and not clamp/unclamp on every rotary move

[crazy^millman]

 I know this su#@, but I use a manual entry with unlock codes before the 5 axis operation

and a manual operation with the lock codes after the operation, because if you manually

unlock the rotaries you have to manually lock them or else they wont lock.

 

 

You can make a trigger in the post for look for 5 Axis operations and have it output that code for you. Make a save process for look for it if is called and then turn it back off when the 5 axis operations are done for a tool. I am sorry, but I would rather the post do the heavy lifting here than me having too.

[Guest]

John,

 

Here's an NC Format for you for CAMplete. Shoot me an e-mail. I can walk you through adding it to your NC Format list.

 

THis is what I use. Has TCP, WSEC, TWP and the high speed modes. THe NC Format Editor is what everybody wishes Mastercam's post editor was... WYSIWYG. :

 

Oh, I use Default Mill because it runs unrestricted. I don't use a 5-Axis MD/CD. No need. :

 

There's a few settings you'll need to set up in CAMplete in Tools, Options, File I/O that do not come set up from CAMplete. Let me know when you're ready and I'll get you going faster than anyone... well, maybe not faster than the CAMplete guys but, certainly faster than your dealer. :

 

Edited to remove file.

[Pitka_Guru]

We have a 2014 VF4 with a TR210 that we do simultaneous porting with and this never happens to us, at least not yet.

[Guest]

Unless John has downloaded it 3x... @ you!

 

That file is specific to CAMplete TruePath, it's not readable in anything else.

[MotorCityMinion]

OT.

 

Would anybody care to share information on where to get some training / help files, videos, or of any help forums for Camplete other that what's given at their website?

[Guest]

OT.

 

Would anybody care to share information on where to get some training / help files, videos, or of any help forums for Camplete other that what's given at their website?

Your 1st line is your machine tool dealer. Next would be the builder. Then CAMplete directly. They prefer to have their declares support the product so they can devote the maximum amount of resources to product development. After that... ME.

 

Or you can ask me anything you want. Chances are, the only guy that knows more about it than I do works at Methods, or the guys at CAMplete directly. I've been using it for coming up on 8 years in May or June. I forget.

 

The one thing I struggle with is macros. The rest, I have a pretty good handle on. Especially with regards to interfacing it with Mastercam. That, I have a real good handle on.

[?Mark]

I far prefer the MAM72 I am programming for but I had to do something for our other shop, plus I am working out a new functioning post processor as they have never had one

 

They've been typing in the positioning for years......no more

Is this the company I told you about some 4-5 years ago that you work for now?... I gave them your contact info then. If i remember right, they typed the rotations in comments....the horror!!!

 

Great guys though.

[Guest]

Is this the company I told you about some 4-5 years ago that you work for now?... I gave them your contact info then. If i remember right, they typed the rotations in comments....the horror!!!

 

Great guys though.

That would be an affirmative Mark

 

So far I have a MAM72 post that posts clean, no editing required which has been proven out in simultaneous as well to this point....

 

Now I am working on 5ax Haas post so that no further editing is required and hand coding is required, just about there I think......

 

Likely a short term thing anyway as by all accounts these Haas machines are on their way out

[Guest]

Final update on this

 

The unlock code worked perfectly fine

 

Not sure what the previous issues were but I have a post now that does what is necessary for these machines