[jbcourt]

The router is a Mulitcam 3000 series (see pix).

Tool changer


This machine does not read G like our others machines and the guys on the floor are not happy about it. But the boss wanted it and I need to make a header in the programs I post. Which the Post dosent do now.

For example:
Our haas post has pop ups that ask for the drawing REV and PL program name and programmer name. ect when you click the post button in the mastercam operations manager. And the programs come out looking like the one below.

O06611 ( 149U1760-9 REV- 5-AXIS PROVEN)
N1 ( DATE 13-07-11 TIME 11:10 )
N2 ( MCX- 149U1760-11 REV- 5-AXIS .MCX-5 )
N3 ( NC= 149U1760-11 REV- 5-AXIS .NC )
N4 (DRAWING INFO/DATA )
N5 (PARTS LIST INFORMATION/PL-A )
N6 (OPERATION DESCRIPTION/5-AXIS )
N7 (PROGRAMMER NAME/SEAN/J)
N8 (****************************************)
N9 ( G54 )
N10 ( XY0 = C.L. OF ROTATION )
N11 ( Z0 IS AT THE/C.L. OF ROTATION)
N12 ( MATERIAL SIZE =9.0X8.0X4.5)
N13
N14 ( T1 2.0 FACE MILL 90DEG /4.5 CL)
N15 ( T3 1.25 STARCHIP RUFF /4.0 LOC OOH)
N16 ( T2 1.0 SWIFT FINISHER /4FLT/4.125LOC/4.75 OOH)
N17 ( T4 1.0 INCERT RUFF/.250 RAD/3.0LOC/3.5OOH)
N18 ( T5 .75 BALL /1.0 LOC /3.375 OOH)
N19 ( T6 .75 2FLT BULL .125 RAD/1.625LOC/3.15OOH)
N20 ( T7 .5 90 DEG SPOT DRILL)
N21 ( T8 .531 JOBBER DRILL / 3.5 OOH)
N22 ( T9 .5 EXT FINISH /.75 LOC/3.0 OOH)
N23 ( T10 .75 FINISH BULL .19R/2.3 LOC/3.1 OOH)
N24 ( T11 .5 2FLT BALL FINISHER/.75LOC/3.375OOH)
N25 ( T12 .375 JOBBER DRILL /3.5 OOH)
N26 ( T13 .75 FINISH BULL/.25RAD/2.75LOC/4.OOH)
N27 ( T14 .375 BULL FINISH .06R/.625LOC/2.1OOH)
N28 ( T15 .375 BALL FINISH/2FLT /.5LOC/2.5OOH)

The programs for the Multicam router post out looking like this:
M90
G90
G70
G75
G97 S15000
G00 T8
( .1875 DRILL/FOR SCREWS )
G00 Z-2.
G00 X-1.1608 Y47.0197
M12
Z-.12
G01 Z.07 F.83
G00 Z-.12
X-17.1631
G01 Z.07 F.83
G00 Z-.12

I see the where the variables are at in the Haas post for the Information to be ented and gathered for drawing REV and PL program name and programmer name. ect but dont know how to get the router post to do it.


What will you need to help me? I can send copy of the posts and anything else you need.

[txcncman]

I use X3, but I can give it a shot and try to walk you through it if you can't find any other support.

Start trying all of the available Machine Definitions and Control Definitions and Post Processors you have and find the one that outputs G-code closest to what is needed.

Then make copies of that Machine Definition, Control Definition, and Post Processor and rename them MULTICAM 3000 ROUTER, keeping the appropriate extensions.

Open MasterCAM and under Settings, open the Machine Definition Manager. Select Machine Type to Open - Router. Then open your newly created router, MULTICAM 3000 ROUTER.rmd. Change the control definition to your newly created control, MULTICAM 3000 ROUTER.control. Open the Control Definition dialog and change the post to your newly created MULTICAM 3000 ROUTER.pst.

Once you complete these steps, message back and I will try to walk you through editing the post processor to change the G-code that is output as needed.

[jbcourt]

Let me be more clear. Mastercam ahas given us a Post that works for the router. But the post doesnt make a header. I want help editing the post to make a custom header.

The reason why I just dont ask symtec to help me with it is because I want to learn how to do it myself.

[txcncman]

If you don't know how to get through the above steps in MasterCAM, we may have to back up and review some basics. If I do not reply here in a reasonable time, email to [email protected]. Sometimes I will get the message quicker. Considering this is the weekend, I probably won't be at the computer as much as on weekdays.

What is your time line for getting this up and running?

[jbcourt]

No rush, the Post processor for the router works just fine, I can enter the program info in manually for now.

Will I still need to go though the step you laid out to make the Post Processor out put header info?

[txcncman]

Oh, and if you haven't yet, review the Multicam parameter specs at MultiCam - Support - M & G Codes.

[txcncman]

Well, maybe I misunderstood what you were really needing. If your G-code works fine, then it is possible in MasterCAM to enter Manual Entry under Toolpaths. Just enter the data you want "As Comment" at the first process. See screen shots attached.

[txcncman]

How much header information are you really needing? When manually g-coding, I usually include:

(Part number and info and date)
(Material blank info)
(Work zero info)

[txcncman]

Finally, to wrap this up for today, to get MasterCAM to automatically post this info, you will have to make a dedicated post processor for this machine and edit it appropriately. I just always go through the steps mentioned above so that everything is wrapped up in a nice little package with one name so when I choose my machine I do not have to run around MasterCAM changing the post processor and such. I do not know of any other work around for your situation unless you purchase a pre-made post processor for MasterCAM. Last I heard, I think I was quoted $800.00 for a custom post processor.

[jbcourt]

Yes txcncman I always use the manual code function when incerting M00 and and toolpath information.

But I want the router post to make a header like the fanuc post for the HAAS's has.

[txcncman]

The part of the post possessor for my Generic Haas VF-TR_Series 5X Mill.pst for beginning the header info is at line 891. See attachment.

Maybe you can zip the Machine Definition, Machine Control, and Post Processor files you are using to a zip file and upload so I can take a look at them.

[txcncman]

Also include a basic MasterCAM part file that we both can use for testing purposes.

[Superman]

O06611 ( 149U1760-9 REV- 5-AXIS PROVEN)
N1 ( DATE 13-07-11 TIME 11:10 )
N2 ( MCX- 149U1760-11 REV- 5-AXIS .MCX-5 )
N3 ( NC= 149U1760-11 REV- 5-AXIS .NC )
N4 (DRAWING INFO/DATA )
N5 (PARTS LIST INFORMATION/PL-A )
N6 (OPERATION DESCRIPTION/5-AXIS )
N7 (PROGRAMMER NAME/SEAN/J)
N8 (****************************************)
N9 ( G54 )
N10 ( XY0 = C.L. OF ROTATION )
N11 ( Z0 IS AT THE/C.L. OF ROTATION)
N12 ( MATERIAL SIZE =9.0X8.0X4.5)
N13
N14 ( T1 2.0 FACE MILL 90DEG /4.5 CL)
N15 ( T3 1.25 STARCHIP RUFF /4.0 LOC OOH)
N16 ( T2 1.0 SWIFT FINISHER /4FLT/4.125LOC/4.75 OOH)
N17 ( T4 1.0 INCERT RUFF/.250 RAD/3.0LOC/3.5OOH)
N18 ( T5 .75 BALL /1.0 LOC /3.375 OOH)
N19 ( T6 .75 2FLT BULL .125 RAD/1.625LOC/3.15OOH)
N20 ( T7 .5 90 DEG SPOT DRILL)
N21 ( T8 .531 JOBBER DRILL / 3.5 OOH)
N22 ( T9 .5 EXT FINISH /.75 LOC/3.0 OOH)
N23 ( T10 .75 FINISH BULL .19R/2.3 LOC/3.1 OOH)
N24 ( T11 .5 2FLT BALL FINISHER/.75LOC/3.375OOH)
N25 ( T12 .375 JOBBER DRILL /3.5 OOH)
N26 ( T13 .75 FINISH BULL/.25RAD/2.75LOC/4.OOH)
N27 ( T14 .375 BULL FINISH .06R/.625LOC/2.1OOH)
N28 ( T15 .375 BALL FINISH/2FLT /.5LOC/2.5OOH)

Technically, they are all comments outputs

The orange section output located in the pheader$ section

The green section is part of the answered questions & may also be part of the pheader$

The purple section may be a Manual Data Input as a comment

The Blue section is the toollist, it needs to be enabled in the upper section of the post
( look for the following & set the same)
-----tool_table : 1 #Tool table, 0=no, 1=yes, 2=Predator VCNC, 3=MetaCut View ( this sets the output format of the info )
-----tooltable$ : 1 #Read for tool table and pwrtt - use tool_table to disable ( this enables the output at the top of the NC file )
pwrtt$ is the string to actually write the toollist, and should be placed up near the top of the psof$ section before safety code outputs

Some older posts do not have this, it needs to then be incorporated into those posts ( there is more than just these lines of info )

There are a couple of ways to have a header:-
1/- have a basic "skeleton Header" hard coded into the post, but the required data would need inputting every time it is posted.
2/- the one that txcncman mentions, to place the text into the upper box to be output as a comment - restriction is the amount of text characters it can handle, a plus - is the text entered is there for each posting
3/- similar to the last, is to call in a TXT file into the Manual Data Operation and have it output as a comment - no restriction on the number of characters
( we saved our TXT files in a dedicated network folder, but placed a link in the location that mastercam takes us to when loading that TXT file, we then made the link folder write protected so that no info was actually saved in the local directory )

The generic post would need tweeking the placements of these "comments" to suit your end needs on which direction you take.

[jbcourt]

txcncman sorry I was gone for a bit, went to see the movie "Contagion" with my daughter. Great movie!

Yes I will gather up the things you requested.

[jbcourt]

Superman, thank you. BTW the text you colored blue is gathered mostly from Mastercam. The out of holder and lenght of cut info is entered by me after post processing.