Using a tool as a stop

[Darin]

What is the correct way to take a tool with a dowel pin in the holder and use it for a stop? I created a point where I wanted the tool to go and used tool path point. But after I do this it asked for a type of tool and there is not stop. So I selected a drill called it 3/8 dia like my pin. But it needs speeds & feeds which I don't want to put in. Also I want it to M00 with the tool... So I selected in the canned text... add stop with tool. But it posts like this. I don't think you can have two M codes on the same line. How do you guys do it?

 

 

N100 G20

N110 G0 G17 G40 G49 G80 G90

( MPMASTER GENERIC 3/4-AXIS VERTICAL )

( MACHINE GROUP-1 )

( 3/8 DOWEL FOR POSTIONING )

N120 T5 M6

N130 G0 G90 G54 X-1.25 Y3.075 A0. S100 M3 M00

N140 G43 H5 Z0. T1

N150 M5

N160 G91 G28 Z0.

N170 A0.

N180 M01

( MPMASTER GENERIC 3/4-AXIS VERTICAL )

( MACHINE GROUP-1 )

( MILLS OUTSIDE PROFILE WITH 3/4 ENDMILL )

N190 M8

N200 T1 M6

N210 G0 G90 G54 X.5 Y-3.25 A0. S7500 M3

[BenK]

I normally just hand edit a drill point to look something like this.

I always like to add notes at an M0 to let the operator know what they need to do.

 

 

 

 

N100 G20

N110 G0 G17 G40 G49 G80 G90

( MPMASTER GENERIC 3/4-AXIS VERTICAL )

( MACHINE GROUP-1 )

( 3/8 DOWEL FOR POSTIONING )

N120 T5 M6

N130 G0 G90 G54 X-1.25 Y3.075 A0. <--------

N140 G43 H5 Z0. T1 <---------

N150 M00 <---------

(POSITION AND CLAMP PART) <--------

N160 G91 G28 Z0.

N170 A0.

N180 M01

( MPMASTER GENERIC 3/4-AXIS VERTICAL )

( MACHINE GROUP-1 )

( MILLS OUTSIDE PROFILE WITH 3/4 ENDMILL )

N190 M8

N200 T1 M6

N210 G0 G90 G54 X.5 Y-3.25 A0. S7500 M3

[Darin]

I normally just hand edit a drill point to look something like this.

I always like to add notes at an M0 to let the operator know what they need to do.

 

 

 

 

N100 G20

N110 G0 G17 G40 G49 G80 G90

( MPMASTER GENERIC 3/4-AXIS VERTICAL )

( MACHINE GROUP-1 )

( 3/8 DOWEL FOR POSTIONING )

N120 T5 M6

N130 G0 G90 G54 X-1.25 Y3.075 A0. <--------

N140 G43 H5 Z0. T1 <---------

N150 M00 <---------

(POSITION AND CLAMP PART) <--------

N160 G91 G28 Z0.

N170 A0.

N180 M01

( MPMASTER GENERIC 3/4-AXIS VERTICAL )

( MACHINE GROUP-1 )

( MILLS OUTSIDE PROFILE WITH 3/4 ENDMILL )

N190 M8

N200 T1 M6

N210 G0 G90 G54 X.5 Y-3.25 A0. S7500 M3

 

 

Ya that is how I do it now. I just would like it to be able to post like that. Mostly because I have alot of jobs that could use this.

Thanks

[BenK]

Just create a text file and use a manual entry. If you do it a lot that probably be the fastest way.

[K2csq7]

I use a point toolpath for tool length offset checks, it comes out looking like this...

N100 G00 G91 G28 Z0.
N110 G00 G17 G20 G40 G49 G80 G90 G94 G98 H00
N120 T237 M06
N130 M00
( CONFIRM T237 H237 D237 DIA = 0.3750 )
N140 M21 (UNLOCK C)
N150 M11 (UNLOCK 
N160 G00 G17 G90 G54 C0. B0. X6. Y0. S100 M03
N170 M20 (LOCK C)
N180 M10 (LOCK 
N190 G43 H237 Z3.
N200 G94 G01 Z2. F20.3
N210 M00 (2.0 FROM TOP OF PART TLO CHECK )

N220 G00 G91 Z15.
N230 G90 H00
N240 M30
%

 

I think this would work for you, let me know if your interested and I will show you the 2 post mods to make it happen.

[Mic6]

Just create a text file and use a manual entry. If you do it a lot that probably be the fastest way.

 

^this

[crazy^millman]

Man are you guys really thinking that far outside of being able to simulate your toolpath? (Old-Forum Head Scratch) Use a drill point tool path. Define yourself a custom tool with no spindle speed. Then like suggested you could do a dimple post mod and have it not put out spindle speed command pretty easy. By making it a toolpath you have something you can see in simulation. Now if you want to create a simulation path that can be shared it will show the stop coming down and the part running from there. I would strongly suggest the point toolpath, since you now have toolpath control over where you want the stop relative to your part in Mastercam and not wondering if you know where you want it using a txt file.

 

HTH

[Tinhman]

Or you can try this and you are good to go from now on.

Custom one "special drill cycle" for it.

 

Code

-----------------------------

if drillcyc$ = 11,

[

z$ = refht_a

pxout, pyout, z$, "F120.", e$

pfzout, "(PUSH PART AGAINST STOP)", e$

z$ = initht$

*z$, e$

]

--------------------------------

Never try this but it should work.

 

HTH

[jeff]

As mentioned above, a text file is the fastest way that I have found.

And you can save it so it's the same with all programs which makes editing a lot easier.

[Trevor Bailey]

custom drill cycle.

[Slepydremr]

Point toolpath.

Manual entry (as code)"M00 (LOCATE PART)"

Point toolpath for retract.

[Roger Martin from CNC Software]

I don't do posts anymore, but I did 'em for 13+ yrs for Mastercam and for 3 yrs before that for "another" product.

 

Listen to Trevor & Tinhman => "Custom Drill Cycle".

 

Just create a text file and use a manual entry. If you do it a lot that probably be the fastest way.

Fast & easy => yes.

The "cleanest" solution => not really.

[jeff]

I've never messed with custom drill cycles as I didn't know how to get it to do what I wanted.

But after seeing Tinhman's example,it looks to be the better option.

Thanks for the example!

[Tinhman]

I actually just added it on my post.

 

Code

-----------------------------------------------------

if drillcyc$ = 18,#DOWEL PIN GUIDE STOP

[

"G01", pxout, pyout, pfzout, pcout, "F120.", e$

"M00", "(PUSH PART AGAINST STOP)", e$

]

------------------------------------------------------

 

This is what i got:

 

N124 ( 1/2 DOWEL PIN)

G0 G17 G40 G80 G90 T124

G0 G28 G91 Z0

G90

M06

(MAX - Z3.)

(MIN - Z-1.)

G00 G17 G90 G54 X0. Y0. S0 M05

G43 H124 Z3. T119

G94

G01 Z-1. F120.

M00 (PUSH PART AGAINST STOP)

M05

G0 G91 G28 Z0.

M01

(*)

[chip]

Could you move the canned text to a different line also?

[Bryan Johnson]

I use the "Stock Advance" toolpath.

You can setup your post to output as needed.

 

see post line

 

pstck_bar_fd$

 

 

 

 

[Darin]

I actually just added it on my post.

 

Code

-----------------------------------------------------

if drillcyc$ = 18,#DOWEL PIN GUIDE STOP

[

"G01", pxout, pyout, pfzout, pcout, "F120.", e$

"M00", "(PUSH PART AGAINST STOP)", e$

]

------------------------------------------------------

 

This is what i got:

 

N124 ( 1/2 DOWEL PIN)

G0 G17 G40 G80 G90 T124

G0 G28 G91 Z0

G90

M06

(MAX - Z3.)

(MIN - Z-1.)

G00 G17 G90 G54 X0. Y0. S0 M05

G43 H124 Z3. T119

G94

G01 Z-1. F120.

M00 (PUSH PART AGAINST STOP)

M05

G0 G91 G28 Z0.

M01

(*)

 

 

Great thanks. So I just add this anywhere to my post? Then select what option in my canned text for this to work? Also how do I control my z depth with this? Tool path point has no option for z depth. Even when I put the point down in z it still posts Z0.

[BenK]

Have you had any Mastercam training? Post edits aren't something for a beginner in my opinion. With some of the questions you have been asking on here it sounds like some classes at your local reseller or tech college would really help you.

[Darin]

Have you had any Mastercam training? Post edits aren't something for a beginner in my opinion. With some of the questions you have been asking on here it sounds like some classes at your local reseller or tech college would really help you.

 

 

Ya thanks. I think I will ask the owner if I can do that. We are swapped here and have to much work right now...hard to find time. I have been a programmer for 20 years but I keep going from Esprit,Gibbs,Catia BobCad,SurfCam,SmartCam. Most of my experience is Solidworks & Esprit. Been out of MasterCam programming for about 8 years. Only been doing it here for about 1 month. Got 150 jobs out so far with it. I also have Matrix Cam in the picture here. Mostly need post work and multi spindle machine help and the new 5 axis we are getting.

[Tinhman]

No i did not use canned text.

Find this section in your post and add it on.

 

--------------------------------------------------------

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

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

.

.

.

------------------------------------------------------------

 

Then change text in drill drop down cycle

 

--------------------------------------------------------------

[drill cycle 18]

1. "Dowel Pin Guide Stop"

2. ""

3. ""

4. ""

5. ""

6. ""

7. ""

8. ""

9. ""

10. ""

11. ""

------------------------------------------------------------------

After change text, you should re-start your mastercam and This cycle should appear on your drill drop down list.

 

 

"how do I control my z depth with this"

 

You should use it like a regular drill toolpath. Draw a point on the screen and pick it for XY location, then enter Z depth in drill parameter page.

that is all

HTH

[Darin]

No i did not use canned text.

Find this section in your post and add it on.

 

--------------------------------------------------------

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

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

.

.

.

------------------------------------------------------------

 

Then change text in drill drop down cycle

 

--------------------------------------------------------------

[drill cycle 18]

1. "Dowel Pin Guide Stop"

2. ""

3. ""

4. ""

5. ""

6. ""

7. ""

8. ""

9. ""

10. ""

11. ""

------------------------------------------------------------------

After change text, you should re-start your mastercam and This cycle should appear on your drill drop down list.

 

 

"how do I control my z depth with this"

 

You should use it like a regular drill toolpath. Draw a point on the screen and pick it for XY location, then enter Z depth in drill parameter page.

that is all

HTH

 

 

Wow ..thanks that worked awesome. The only thing I can't figure out is how to change the text in the drop down menu? Is that in the post?

[Roger Martin from CNC Software]

The only thing I can't figure out is how to change the text in the drop down menu? Is that in the post?

It is, but editing the post text in the PST is not the suggested method, unless you really know what you're doing.

No, you're not going to damage the Post, unless you really screw up!

*You do always make a backup copy of the PST before making any edits - correct?

 

The "proper" way to to alter the Text from within the Control Definition, which will then update the Text in the PST properly.

See my posts (#2 & #10) in this topic --> Can I Rename Drill Cycles?

[crazy^millman]

I would strongly recommend you listen to Roger. He might be long in the tooth like the rest of us, but he knows what he is talking about.

[Darin]

It is, but editing the post text in the PST is not the suggested method, unless you really know what you're doing.

No, you're not going to damage the Post, unless you really screw up!

*You do always make a backup copy of the PST before making any edits - correct?

 

The "proper" way to to alter the Text from within the Control Definition, which will then update the Text in the PST properly.

See my posts (#2 & #10) in this topic --> Can I Rename Drill Cycles?

 

 

Thanks Roger....Worked perfect. I always back up my .pst files so if I make a bad .pst I can go back. I am getting this slowly. Thank for everyones help I really appreciate it.

[Tinhman]

Thanks for a good advice!

Happy Friday.