M00 , program stop

[connormac]

I have to reposition parts and need to know the easiest way to put a program stop ( M00 ) without having to edit it in every time I make a change to the program.

[MACHINEMASTERG]

toolpathes,nextmenu,manualentry then enter moo here and what ever else you want to say

[Mgrenier]

You can also use canned test. Just check the canned text button at the lower right corner of the tool parameters page. And Put the M00 you need where you need it.

 

Hope this helps,

[MACHINEMASTERG]

just learned something new (canned text at bottom of page)thanks

[Toolfab]

That is a neat little trick, thanks for pointing that out. Where do you enter the values for the text fields. Do you have any other info on this fuction. I apreciate any imput you could give. Thanks.

[Jeremiah]

Paul-

In our post's, whatever is entered in the "comments" on the main parameters page will come out with the M00, or whatever canned text entry you choose.

 

One other note on "canned text". You should watch the output when using depth cuts or multi passes. It's possible that you will get an M00 on each pass. Or does my post writer need to roll em tighter ?

 

Jeremiah

[Toolfab]

Jeremiah, my text in the comment box also comes out, but in comes out in () these. It comes out in one line width no spaces. Which means I have to go thru every line of code to put in my A rotates. I have to do alot of this

 

G91 A90

G90

G14 J3 N1=_ N2=_

 

So to put those in a canned text would be SWEET. I can find the canned text & I see how to use it put were do you enter the text that you want "TEXT1" to represent. Any help would be appreciated.

[connormac]

Thanks for all the help. I should have been a little more specific on what i needed. What I need to do is pick up a pin. Go down to .500 above the part then put in a M00 , so I can reposition the part and manually drop the pin in a hole. then continue on with a different tool plane. Hope this makes some kind of since on what I'm trying to do. Thanks

[Jeremiah]

Paul-

If I am understanding you correctly you are editing the nc file for your indexes? I don't think using canned text is the best way to do this. If you are using a 4 axis post, it should be outputting rotations for you. What machine and post are you using?

 

connormac-

Are you using a pin in a tool holder as a hard stop? If so, you might want to try using the point toolpath. Go to XYZ and have canned text set to "with".

[connormac]

I'm using a leadwell post that was made for my company. what I do is put in a .750 drill at zero RPM . Zero as depth of cut. Then when I put in the machine I just change G981 line to M00. Kind of a pain but it works. Help !!!

 

Thanks

Kyle

[Toolfab]

With respect to connormac, to whose thread I accidently side tracked, sorry connormac, I will send an email to Jeremiah.

 

[steve f]

connormac, how much experience do you have editing post processors. If you do, one possibility would be to customize your post so that an M00 would be output on any toolpath when misc integer 4 (for example) was set to 1. In your post you could have a conditional branching line that runs a custom postblock that would output an M00 with a spindle orient or no rotation if mi4 was greater than zero. Just an idea.

 

Steve

[Rekd™]

Here's what I've done... Taken one of the un-used drill cycles and created a custom "Tool Stop" routine for it. You select a drill toolpath, select a point, select a tool, (i have an "Undefined" type where I use a 1/4" dowel pin), select "Tool Stop" from CYCLE in the Drill Dialog, and set my depth. The post automatically sets RPM to Zero, and disables FEED. Then when you post it, you get, without any edits..

 

code:

---

 %

O0001

(PROGRAM: UNNAMED PART.NCF)

(JAN 17, 2003 13:42)

(MC9 FILE: UNNAMED PART)

(MATERIAL: NONE)

(TOOL 1: DIA 0.2500 .250 Tool Stop)

(OVERALL MAX Z1.)

(OVERALL MIN Z-.25)

N1 G00 G17 G40 G49 G80 G90 G20

N2 T1

N3 M01

( OPERATION: 1 DRILL )

N4 ( LOCATE PART )

N5 M06(T1: .250 TOOL STOP)

(MAX-DEPTH | Z-.25)

N6 G00 G90 G54 X1.7138 Y2.3628

N7 G43 H1 Z1. M08 T1

N8 X1.7138 Y2.3628

N9 Z-.25

N10 M00

N11 Z1.

N12 G80

N13 M09

N14 G91 G28 Y0. Z0. A0

N15 G90

N16 M06

N17 M30

%

---

It works great because it's ALL generated from MC, no edits at all. My only problem, which really isn't one, is the G80 at the end.

 

I've also got a program stop routine programmed into the Misc Values box for all Toolpath Parameter boxes. It's basically a toggle, 0 or 1 to disable or enable. And when the post reads this, it automatically prompts you for a comment. It has all the needed positioning features to bring the table out, shut everything off etc. Pretty handy.

 

God I love Mastercam, specially after being subjected to Gibbs for so many years!!!

 

'Rekd

[CNCme]

CONNO

 

DO some editing ...save some time

dont be affraid...post editing takes a lot

of time to learn

 

[ 01-17-2003, 08:21 PM: Message edited by: CNCme ]

[connormac]

Hey Guys,

 

Thanks for all the good ideas. Redk up above just told me there is a way to do what I want. But I'm new at MC. I have used a real basic package up until now. So without sounding to stupid could someone please give me a step-by-step method on how to create a custom tool cycle. I need it to come out almost exactly like Redk's but for a Fanuc.

Thanks again!

[Trevor Bailey]

Con......,

 

You may want to post some sample code in here exactly how you want it. Give us something to look at. I think you will find that most(some) of the forum members could make this change with their eyes closed pretty quickly.

 

On a side note though, have you cantacted your dealer for some help?

[steve f]

Connormac,

 

An honest question with good intentions is never a stupid one. Post a sample of code on the forum and some of the changes you'd like and I'm sure you'll get more than one response on how to go about fixing your problem. Like Trevor said, try contacting your local dealer about this. CNC Software and In House Solutions releases how to information about editing post processors so you might want to ask your dealer about something like that as well. Good Luck,

 

Steve

[connormac]

This is what I can do just using Custom Drill Cycle #9

 

%

O1000

(PLEASE REVIEW SETUP SHEET BEFORE PROCEEDING)

(PROGRAM TEST)

(DATE 01-18-03)

(TIME 11:39)

(T1 - Dowel Pin)

G90 G80 G40 G0

T1 M6

( T1 - Dowel Pin )

G54 G0 X.3646 Y1.0723

G43 H1 Z.1

S0 M5

G80

G0 G28 G91 Z0 M19

G28 G91 Y0.

G90 G53 X20.

G90

M30

 

This is what I need. Just add a M00 after I reach Z.1 so I can stop and reposition my part.

 

%

O1000

(PLEASE REVIEW SETUP SHEET BEFORE PROCEEDING)

(PROGRAM TEST)

(DATE 01-18-03)

(TIME 11:39)

(T1 - Dowel Pin)

G90 G80 G40 G0

T1 M6

( T1 - Dowel Pin )

G54 G0 X.3646 Y1.0723

G43 H1 Z.1

S0 M5

M00

( Reposition part to last .250" hole )

G80

G0 G28 G91 Z0 M19

G28 G91 Y0.

G90 G53 X20.

G90

M30

 

thanks for all your help

[steve f]

Connormac,

 

Open up your post processor in Cimco or whatever editor your using. The directory for your post editable file is probably C:Mill9MillPosts(your post name).pst. Run a search for the postblock called pdrlcst or scroll through until you find a bunch of code that looks like this:

 

pdrlcst #Custom drill cycles 8 - 19 (user option)

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

"CUSTOMIZABLE DRILL CYCLE ", pfxout, pfyout, pfzout, pfcout, e

pcom_movea

 

Change the line that starts with "CUSTOMIZABLE DRILL CYCLE" to read n, "M00", e and it should look like the following:

 

pdrlcst #Custom drill cycles 8 - 19 (user option)

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

n, "M00", e

pcom_movea

 

This should get you what your after and if it doesn't post the result on the forum and I'll help you out.

 

Steve

[steve f]

Rekd,

 

To get rid of the G80 in your custom "Tool Stop" cycle, edit your pcanceldc postblock to look like this:

 

pcanceldc #Cancel canned drill cycle

result = newfs (three, zinc)

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pxyzcout

!zabs, !zinc

prv_gcode = zero

pcan

if gcode >= 8, pcan2

else,

pcan1, pbld, n, "G80", strcantext, e

pcan2

 

This is for a standard MpFan post but it might give you an idea of where to look if you have a different post.

 

Steve

[Rekd™]

Thanks, Steve.

 

I'll check it out Monday.

 

'Rekd

[Bimm]

On 16/1/2003 at 10:20 AM, Toolfab said:

Geremia, anche il mio testo nella casella dei commenti esce, ma in esce in () questi. Esce in una sola riga senza spazi. Il che significa che devo passare attraverso ogni riga di codice da inserire nel mio A rotates. Devo fare molto di questo

 

G91 A90

G90

G14 J3 N1 = _ N2 = _

 

Quindi mettere quelli in un testo in scatola sarebbe DOLCE. Riesco a trovare il testo in scatola e vedo come usarlo messo sei entrato nel testo che vuoi "TEXT1" per rappresentare. Qualsiasi aiuto sarebbe apprezzato.

good evening
would you kindly have this Philips post?
Thanks for your help

[crazy^millman]

48 minutes ago, Bimm said:

good evening
would you kindly have this Philips post?
Thanks for your help

Asking for post is not allowed on this forum. Contact your dealer and they can provide you with one.