MPLFAN post processor

[victor nguyen]

Hi!

Please! some one tell me How can I edit the starting up program as the way I want on the

MPLFan ,lathe packet MC9.1 . I swithed around cimcoedit and other, but starting up program was the same .

Because ,many machine's program start up is difference , I have to edit each tool , and trim unnessary G code and G01 place on Z- line insead Z+ as MPLFAN does . The MPLFAN start up only one style , I want to set each machine have starting up as I want when post it and I do not edit each line .

It would be nice to have trim and neatly program , Any helps will be great of my apreciation

[Hardmill]

How about showing us how the code looks and how you

want it to look.

 

 

PEACE

[victor nguyen]

Ok , I typed them below

(rough tool )

GO T0101

G97 S275 M03

G00 G54 X6.250 Z.1 M08

G50 S1250

G96 S450

G99 G01 Z0.F.01

Z-6.

That's axactly Mpl fan on my mc9.1

the way I want them below

G0 T0101

G50 S1250

G96 S450 M03

G00 X6.250 Z.1 M08

G01 Z-6. F.006

It's semple like that , most of machine they have the extend home position ,then no need G54

only 2 home position in same program , then need it, G97 option I used for center drill or drill ,

if there is option I can switch G96 or G97 is the best ,spacially on G01 place right on z-6. line , if it place on Z0 or Z.1 it cut on the air ,and the groove cut back out , it just straight back out better move one side then bakc out and we have one more axtra line , one program there many axtra line move like this

It will confuse the operator . I would be better if we have more option starting up program for older machine or new machine or custom starting up as they want

please helps me fix that , thank you very much

[Mike Whitten CAD/CAM Contractors]

Victor,

 

Have a look at this question in the post if you have it:

 

css_start_rpm : yes #Do direct RPM spindle start prior to CSS ?

 

You may just have to enter a no.

 

Mike

[victor nguyen]

Hi Michael!

Thank you very much , you made one part of them right , I changed csss as you note , the post terminate G97 and all it's line as rpm and M03 .

Please ! I need some more help ,Please, some one tell me How to edit MPLFan remove G54 from the post? And place G01 right on Z- line instead one line ealier , no need extra line for me , and very tired to edit starting up each tool for 6 or 7 tool for single program , and over 10 cnc lathes machine ,I could not count how many time I have to edit over over again.

Once again I appreciated any helps

[Guest CNC Apps Guy 1]

I hope you use "G0" instead of "GO". GO's going to give you problems.

[Mike Whitten CAD/CAM Contractors]

Victor,

 

There are several ways to get rid of the work offset. I am not sure what would be best for your situation as I don't really know exactly what it is. I believe the following is the most common though.

 

Comments from the mplfan.pst found in V9.1 MR0105 :

 

# mi1 - Work coordinate system: (home_type)

# -1 = Reference return / Tool offset positioning.

# 0 = G50 with the X and Z home positions.

# 1 = X and Z home positions.

# 2 = WCS of G54, G55.... based on Mastercam settings.

 

I believe that you may just need to set mi1 to -1 or 1 depending on whether you are using TC positions or G28 home

 

 

I am not sure about the Z issue as I would like to look at a file.

 

Ooh! by the way, I am not a MC Lathe or Lathe post Guru. I am just trying to help, so if someone sees an error or has anything to add or change, please feel free help us out.

 

Thanks,

Mike

[terry5357]

+1 Micheal a post is a post is a post......most of the time. you have him headed in the right direction.. good job

[victor nguyen]

HI

I set mil-1, but not work G54 still there , not things changed after post .

[Mike Whitten CAD/CAM Contractors]

Victor,

 

I tested it with a post from MR0105. The modified date (Windows) on the post I have is 1-24-05. and the txt file is 2-4-03

 

TXT file entries:

 

[lathe misc integers]

1. "Work Pos. [-1=REF,0=G50,1=HOME,2=G54s]"

2. "Abs/Inc. [0=ABS, 1=INC]"

3. "Ref. Return [0=G28,1=G30]"

4. "Misc. integer [4]"

5. "Misc. integer [5]"

6. "Misc. integer [6]"

7. "Misc. integer [7]"

8. "Misc. integer [8]"

9. "Misc. integer [9]"

10. "Misc. integer [10]"

 

I do not know what post you have. ?? Maybe someone changed it or maybe it is very old and does not support this. Can you find one on your install CD ??

 

Mike

[victor nguyen]

hi Mike

I have post MR0304 and lathe Misc integger as below

-1=ref return/tool offset pos

0=G50 with X and Z home pos

1=X and Z home pos

2=WCS G54, G55 ... base on MC setting

I changed -1 to 1 for ref return/tool offset,

Then posted again , But it does not work , G54 still in there and G01 still created extra line instead pleace G01 right on ( G01 Z-6. or whatever Z- negative sign ) intsead

G01 Z0.

Z-6.

Please ! Some one tell me how to get grid G54 as option , And pleace G01 and feed rate are right on the starting cut line as (G01 Z-6. F.01)After you post every time . Thank you

[victor nguyen]

Hi

I found the way to set coordinate , but could not get grid of G54 , because the sofware creator did not put on the post . MC default

-1=G54 , 1=G55,2=G56 , if I set 0 , or -2 It's still G54 .Is there any body know How scrip or add more # on the MPLFan to get grid G54 after post?

Any helps will be great .

[Guest]

To completely get rid of any G54,G55,G56, go into the ltlchg$ section of the post adr remove

 

code:

---

pcan1, pbld, n$, psccomp, *sgcode, pwcs, pfxout, pyout, pfzout,

pscool, strcantext, e$

---

The pwcs from the line.

 

once you do that you will not get anymore G54 at all or be able to change it except by editing.

 

Is that what you are looking to do?

[victor nguyen]

HI!

Thank you John , I just found anather way by select (misc value and set Work pos to 0 , then G54 gone , Default is 2)

I need one more help on G28 (reference home )

Some one tell me How set (G28 ref home) after post it's G28 U0 only , instead G28 U0 W0 . Because some machine got long bed , it's wasting time to all the way home , then back forward for next tool , I just move out a few inches , then starting next tool .

Programmer's rules is very trict to save their job , doing axactly the way they want .

Is there any body know how to set G28 U0 only after post instead G28 U0 W0? Please , tell me , Thank you .

[Ashan]

pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.", e$

 

 

I think on this line just remove "W0"

IT will do

[victor nguyen]

Hi Ashan

please , can you tell me more spacific detail ,

how to get to pbld,n$,*sg28,"U0",(if Y-axis-mch.......) . Or Do you mean manually edit by hand each tool ? Thank you

[Ashan]

pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.", e$

 

Yes on each lines on post

[Ashan]

pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.", e$

I think 4 places on post

You shoud remove "W0.",

[victor nguyen]

Hi!

thank you very much for quick responding , I found the in the MPLFan post ,It's under (Start OF File and Tool Change set up ) please , tell me how to edit , what's part of the line tobe deleted ?

 

[ 09-13-2006, 02:01 PM: Message edited by: victor nguyen ]

[victor nguyen]

Hi

if I deleted "W0." on that line , I've got error as

Combined Mill and Lathe Post Processor Version 9.19 © Copyright 1992-2004 CNC Software, Inc.

Processing file with MPLFAN...

Variable not defined:

Post line number 1256

Program execution halted due to error(s) in .pst

[Guest]

Victor,

 

I think perhaps a call to your reseller is in order.

 

They should be able to get you straight in fairly short order.

[victor nguyen]

Hi John !

I'm sorry John , I'm missunderstanding what to oder from my reseller MC9 ? Is that some thing add on to my MC9? please, tell me little more specific , Thank you

[victor nguyen]

Hi John !

I talked to my local reseller , He is Ok to help me on edit the post , I will send him the problem , but not warranty the problem solve .

I still need some one help out there , please , thank you .

[Ashan]

problem Is $ If it is version 9 post

remove all $ sign every where

as below

pbld, n, *sg28ref, "U0.", [if y_axis_mch, "V0."], e

[victor nguyen]

Hi

that's 9.1 mC9 . there are any $ sign on that line , It's axactly as you tiped

pbdl,n,*sg28ref,"U0."(if y_axis_much, "v0."),"W0.",e

It've erro when I deleted "w0."

What more will i do ?