M00 to post

[C JAYNES]

How can I create an M00 in my program using Mastercam. I often have the need to insert a M00 in my programs in order to move clamps and ect. I have tried using manual entry, but in the code it comes out in parenthesis. I could just delete these, but I am trying to eliminate manually editing my programs.I am using a Haas post. Ideally I would like to be able to have Mastercam post the M00 and have the table return to the Y and Z home postion. Thanks in advance for your help.

[Jeremiah]

this is a post block that we call with mi3

 

pstop_restart

prv_coolant = 0

if opcode = 15,

[

sav_xout = vequ(xout)

xout = vequ(x)

n,G00,*zout,e

n,pwcs,*xout,*yout,e

n,M00,comment,e

n,pchg_speed,*spindle_on,e

pcoolant_on,e

xout = vequ(sav_xout)

]

else,

[

sav_xout = vequ(xout)

xout = vequ(xh)

n,G00,*zout,e

n,*xout,*yout,e

n,M00,comment,e

n,pchg_speed,*spindle_on,e

pcoolant_on,e

xout = vequ(sav_xout)

]

 

it is for stopping and restarting with the same tool. uses home position.

 

Good luck.

Jeremiah

 

[ 04-24-2003, 10:28 AM: Message edited by: Jeremiah ]

[connormac]

What I did was went into the post and changed Misc. Drill #2 to Tool Stop. You can use this for part reposition and to move clamps. It works pretty well. If you want I'll try to remember exactly what I did. But I may have to wait till I get to work and look on my laptop.

[Rekd™]

I set my post up to use Misc Values where I can flip a switch on any operation and it will post an M00 at the beginning of that operation. It will also prompt you for a comment to add to the output.

 

'Rekd teh Don't be shy... close your eyes and push the big green button!

[Rekd™]

Here's what I use..

 

Post.txt file:

code:

---

[misc integers]

<snip>

10. "M00 before operation [0=No,1=Yes]"

</snip>

---

Post.pst file:

code:

---

# mi10 - M00 before operation. If stop is set with same tool as previous

# operation, tool change values will be posted before and

# after the stop. The post will prompt for a comment when a

# stop is found, and that comment will print to the nc file.

# 0 = No (Default)

# 1 = Yes

 

 

# User Defined Questions

# --------------------------------------------------------------------------

fq 3 stopcomment M00 found for: //t//; //strtool//. Enter a Comment...

 

 

pstop # Stop routine

pretract

q3 #Stop Comment?

stopcomment = ucase(stopcomment)

if stopcomment = "", n, "M00", e

if stopcomment <> "", n, "M00", "(", *stopcomment, ")", e

if wcstype > one, absinc = zero

n, *spindle, *speed, pgear, strcantext,e

pcan1, pbld, n, *sgcode, *sgabsinc, pwcs, pfxout, pfyout, pfcout, *cabs, e

pbld, n, "G43", *tlngno, pfzout, scoolant, next_tool, e

absinc = sav_absinc

 

 

ptlchg #Tool change

<snip>

if mi10=one,

[

pbld, n, "G91", "G28", "Z0.", e

pbld, n, "G91", "G28", "Y0.", e

pbld, n, "G90", e

q3 #Stop Comment?

stopcomment = ucase(stopcomment)

if stopcomment = "", n, "M00", e

if stopcomment <> "", n, "M00", "(", *stopcomment, ")", e

</snip>

 

---

I also have a drill cycle set up for a tool stop like Kyle. Works great. I've also got cycles that do Deep Hole Drilling using IJ and K instead of Q, I've got one that lets you generate a sub program call, and one that does a Serialized Engraving or a String Engraving cycle. Very cool stuff, but I'm not going to give any of my 1337 drill cycles away.

 

'Rekd teh Lets See Gibbs Do That!

[FUSION]

Hey C Jaynes, why dont you contact your buddies in Cal. Namely the two that work at the mold shop.This is J.H. Write me back @ my e-mail address. You should be able to use the little icon on this reply.

[iowajim62]

Hi CJaynes,

 

quote:

---

but in the code it comes out in parenthesis

---

To remedy this go to your manual entry and change NCI output method from 1005 to 1006. It will post without ().

HTH

[C JAYNES]

Thanks everyone J.H. check your email. Iowa Jim thanks but that did not work. I tried both settings.

[Smit]

In the MPMaster post (available for download on this web site), changing mi10 to 1 will output the M0 before the operation. I use the MPMaster for all of our 3 axis machines here, it works very well.

[Thad]

quote:

---

'Rekd teh Lets See Gibbs Do That!

---

Rekd,

 

If Gibbs sucks so bad, how come you continue to use a Gibbs screen shot in your avatar?

 

Thad

[Rekd™]

quote:

---

If Gibbs sucks so bad, how come you continue to use a Gibbs screen shot in your avatar?

---

Uh oh.. Here we go again...

 

That's not Gibbs. It's from a plug-in we used with/for Cimitron. (I think the surfcam verify uses the same engine as that plug-in) Cimitron was tough to learn. Powerful but seriously lacking support.

 

Gibbs doesn't "Suck so bad". It's just that it's more for beginners, or those that don't like to be in control. (No offense to any Gibbs users out there)

 

It's big thing is that's it's easy to use, which is true. But try to get it to do exactally what you want and you may be disapointed. And configuration for personal preference is a joke. Post processor???? I think not! (How many times I've sent them a simple change only to have to send it back to fix the 2 other things they messed up while making that 1 change...)

 

I'm thankful for Gibbs. I learned CAD/CAM on the DOS version. I also had the pleasure of using the original GibbsCAD/CAM on a Mac. That was much better than Virtual Gibbs.

 

I've used it off and on my whole programming career. They've got some seriously neat stuff, but nothing I would trade for Mastercam. (Well, there is still the issue of the Geometry Expert, but that's a different thread)

 

'Rekd teh "Peaches come from a can, they were put there by a man, in a factory downtown."

 

[ 04-24-2003, 11:40 PM: Message edited by: Rekd ]

[Guest CNC Apps Guy 1]

I changed pcan2 to look like this;

 

pcan2 #Canned text - after output call

if opcode1 = 3 & dwell <> zero & gcode = one, pdwell1

if cantext = one, pbld, n, "M01", e

if cantext = 2, n, "G00", "G98", "X20.0", "Y20.0", e

if cantext = 2, pbld, n, "M00", e

 

Then I use the STOP in the Canned Text in the toolpath I want to add it to. This moves the table to the front and center of travel on our Cinci POS machines. Also if it is a tool that was used in the previous op, I'll Force a tool change.

 

HTH

[kathy]

This is out solution for 'program stops':

 

 

http://www.emastercam.com/ubb/ultimatebb.p...t=001506#000005

 

Kathy

[Thad]

Rekd,

 

I stand corrected.

 

Thad

[billystein]

This is a good time for canned text. It seems to work fine for things like M00 and M60 and little one code commands.

I have fixed it in the bfad9.pst make sure you get the txt file also.