PostHaste, Rigid Tap, Spindle Speed, Direction

[gr_mich_mush]

Ok, I know this is asking a lot but, if there is a PostHaste god out there I am sure it will be nothing for them to figure out. Of course any help will be greatly appreciated. This is what I am trying to do. I want PostHaste & GibbsCam V8.5 to output a rigid tap code like this. Oh, and I am not trying to yell by putting what I say in bold. It is to distinguish between code and what I am saying. I know all CAPS and Bold annoy some people.


M06
G00G90G43G54H5X0Y0Z1.T15
M08
G00Z0.1
M29S130
G99G84R0.1Z-1.F10.
X1.Y1.
G00Z1.


Our Machine requires that the intro line has no spindle speed or direction in it.
So first I put this in PostHaste

Tap Tapping cycle
M29 S[Speed]
G[RetPlane] G84 R[RLevel] Z[D] F[Frate]
end cancel

1stToolChange First tool change
G00 G80 G40 G28 G91 Z00 T[Tool] M6
G00 G90 G43 H[Lcomp] G[Work] X[H] Y[V] Z[D] M[Direct] S[Speed] T[NextTool]
M[Cool]
End

ToolChange Secondary tool changes
M6
G0 G90 G43 H[Lcomp] G[Work] X[H] Y[V] Z[D] M[Direct] S[Speed] T[NextTool]
M[Cool]
End

That produces...

M06
G00G90G43G54H5X0Y0Z1.M03S130T15
M08
G00Z0.1
M29S130
G99G84R0.1Z-1.F10.
X1.Y1.
G00Z1.


Note the "M03S130" in the intro line of the drill cycle. That is what I am trying to get rid of.
So I changed sequences to

Tap Tapping cycle
M29 S[Speed]
G[RetPlane] G84 R[RLevel] Z[D] F[Frate]
end cancel

1stToolChange First tool change
IF [Cycle] = [tap]
G00 G80 G40 G28 G91 Z00 T[Tool] M6
G0 G90 G43 H[Lcomp] G[Work] X[H] Y[V] Z[D] T[NextTool]
ELSE
G00 G80 G40 G28 G91 Z00 T[Tool] M6
G0 G90 G43 H[Lcomp] G[Work] X[H] Y[V] Z[D] M[Direct] S[Speed] T[NextTool]
ENDIF
M[Cool]
End

ToolChange Secondary tool changes
IF [Cycle] = [tap]
M6
G0 G90 G43 H[Lcomp] G[Work] X[H] Y[V] Z[D] T[NextTool]
ELSE
M6
G0 G90 G43 H[Lcomp] G[Work] X[H] Y[V] Z[D] M[Direct] S[Speed] T[NextTool]
ENDIF
M[Cool]
End

Then that gives me an error saying...
Internal Error <VC>: Unrecognized Maching Mode in CL File...
Problem on line 14 of CL file...
Error at APPLY / MILL...

Does anybody have any idea how to fix this???
I have included all the files that may shed some light on the issue(CL file, .vnc file, PostHaste templates, and Posthaste Log). Plus if I get this done it will be a GREAT template for other fanuc machines that use M29. And of course I would offer it to anyone that asks.

[gr_mich_mush]

Did I post this in the right section?? I thought I'd get some sorta response...
????????????

[cadman]

I'll take a look at it this weekend. I made all of my templates while I worked for my last employer.

[gr_mich_mush]

Thank You. I'll appreciate any help you can offer. I think I got the idea down but am missing a detail.

[cadman]

The only problem I found was the speed for the tap. You set the spindle clamp at 150 to 12000 rpm, but only had 130 rpm for the tap. Once I changed that your modified template worked fine just like you wanted.

Looking at your CL file, are you trying to post with CS using a standard Posthaste template? This section near the top indicates you are and is probably what is giving you the mode error:

$$-> CS NUMBER 1.
$$-> CSYS / 1.000000000, 0.000000000, 0.000000000, 0.000000000, $
0.000000000, 1.000000000, 0.000000000, 0.000000000, $
0.000000000, 0.000000000, 1.000000000, 0.000000000

To post using CS, you need to purchase the upgrade from Posthaste. The standard Posthaste plug-in only works with up to 3 axis and no CS.

Anyways, I see no problem. I'm using GibbsCAM V9.3.14, but I still would have experienced the same errors if there were any in your template, but it works.

[gr_mich_mush]

Ok, this is really weird. I just tried to recreate the error msg. I was going to take a screen shot of it to show you. But it worked. The only msg I get was the spindle speed warning as you mentioned (that it something I want to stay). I am totally confused now. The only thing I can think of is that the Gibbs and the computer were restarted. But, either way it is working just the way I was trying to get it to. Anyway, on a unrelated note. Which is not near as important. Is there a way to eliminate the "G00Z1." at the end of every drill cycle. Is that something you change in the PostHaste.cfg file?

(TOOL 3)
(13/32 DRILL)
(OPERATION 1)
G00G80G40G28G91M06T03
G00G90G43G54H3X0Y0Z1.M03S893T05
M08
G00Z0.1
G99G81R0.1Z-1.3721F7.
X1.Y1.
G00Z1.
(TOOL 5)
(1/2-13 CUT TAP)
(OPERATION 2)
M06
G00G90G43G54H5X0Y0Z1.T15
M08
G00Z0.1
M29S130
G99G84R0.1Z-1.F10.
X1.Y1.
G00Z1.
(TOOL 15)
(1/2 FINISHER)
(OPERATION 3)
M06

Thank you so much for your help over the weekend.

[cadman]

Look at the cycle cancel line in the template and tab the G0 line over a couple places or delete it.

[gr_mich_mush]

I do not have a G0 in that line. It looks like this.

Cancel
end

From what I can see, the CL file tells it to retract to 1.0000000 three times, at the end.

$$ StartNewTool...
CUTTER / 0.406250, 0.000000, 2.000000
LOAD / TOOL, 3, ADJUST, 3
$$ TOOLID / 3
CUTCOM / ON, LENGTH, 3
SPINDL / RPM, 893.000000, CLW
COOLNT / FLOOD
RAPID
GOTO / 0.0000000, 0.0000000, 1.0000000
$$ ...end StartNewTool.
$$ ...end StartFirstOp.
RAPID
GOTO / 0.0000000, 0.0000000, 1.0000000
RAPID
GOTO / 0.0000000, 0.0000000, 0.1000000
RAPID
GOTO / 0.0000000, 0.0000000, 0.1000000
$$ Starting Drill cycle (DoDrill)...
RAPID
GOTO / 0.0000000, 0.0000000, 0.1000000
CYCLE / DRILL, DEPTH, 1.372100, PERMIN, 7.000000, $
CLEAR, 0.099950
GOTO / 0.0000000, 0.0000000, 0.0000500
GOTO / 1.0000000, 1.0000000, 0.0000500
CYCLE / OFF
RAPID
GOTO / 1.0000000, 1.0000000, 1.0000000
RAPID
GOTO / 1.0000000, 1.0000000, 1.0000000
RAPID
GOTO / 1.0000000, 1.0000000, 1.0000000
$$ StartNewOp...

Either way, you have helped alot. If this is something I have to deal with I can. It was just kinda annoying. I will do some more tweaking to get everything as perfect as I can and then post this as a good Fanuc 16M - 21M template. I am basing this on the last job I had with 3 Leblond Makino w/16Ms and now this job with a NTC w/ 21M. I hope it will help someone. If at some point you can find a way to eliminate that "G00Z1." let me know. Did you see anything else stupid in the template?