Manual entry

[Bolts-and-nuts]

I've recently had an NC program (generated by mastercam v7) which i cant avoid editing manually.

 

My program uses a locating pin used as a tool so that it will be used as a part stopper (to locate the part). To position the pin i used CONTOUR toolpath followed by a MANUAL ENTRY 'M0 (STOP PART USING PIN)'. The produced NC file is what I had expected, The locating pin went to the designated location but returned to the Clearance height then to machine's Z0 before the manual entry appeared.

 

This resulted, as i have said to a manual edit of the NC file where i had to put the manual entry in its right sequence, that is before the pin goes up to the clearance height. I could have lived with editing the NC file, but i made this kind of program for 21 parts this past few days now and my boss told me to expect more. YAIKS!!!

 

Is there a way to avoid this? just to lessen the risks.

 

what if i use V9, would i avoid this problem?

[mayday]

I would build a fixture with a locating pin in it

much more reliable

[Fig sign]

I would wrote a macro .

And when I worked in some other job I do wrote it and used a lot !

Even if it is 6-10 blocks it still has sense if you use it a lot .

 

[ 09-04-2003, 08:09 AM: Message edited by: plasttav ]

[Harryman]

Does your machine have custom macro capability? If so just replace those positions with variables.

 

#100=10. (X STOP POSITION)

#101=3. (Z PIN RAPID POSITION)

#102=1. (Z PIN STOP POSITION)

 

GO X#100 Z#101

Z#102

M00

 

Then just alter the variables to fit the current job.

 

Is this what you have in mind?

[Bolts-and-nuts]

Thanks Mayday for the reply. hmmm.

 

OK, I forgot to add that the setup requires only vise because we only need to make a few pieces/part. the part requires cutting in the right length and its shorter than the vise jaw. i could have put the whole program for the locating pin but as Manual entry but the part has different lengths?

 

using the vise and the locating pin is seems more feasible than using fixture with locating pin hole.

[Bolts-and-nuts]

thanks guys for the replies. I am not used to writing macro and i am not sure wether the machines where they run the program supports macro.

Im in Philippines and they are running the program in Kansas.

 

Does this mean that its not posible producing the NC file in Mcam without manually altering the NC file?

[mayday]

Make your vise jaws out of mild steel and you can cut right thru them and retain your end stop or bolt a stop on the table beside your vice and use a removeable spacer block between your part and your end stop

[Trevor Bailey]

For a pin stop like that, even when working with more than one vise, customize a drill cycle in the post to do this. It works great.

 

Do a search thru the forum. This has been covered before and I believe that Rekd actually posted his format to be copied by anyone.

 

[ 09-04-2003, 08:19 AM: Message edited by: Trevor Bailey, from Barefoot CNC ]

[Fig sign]

Harryman !

I used to add returning by z slope angle so that a pin will has no contact with a part

you must have one more parameter direction

and in return after m0 you add smth like this

(parameter (left)#105=-1)

(Parameter (right)#105=1)

if #105==-1

g91 x-0.1 z2

g90

z2

else

if #105==1

g91 x0.1 z2

g90

z2

else g90 z2

 

Sorry if my macro grammer is wrong I use another

than Fanuc controler

 

Iskander teh tricky

 

[ 09-04-2003, 08:23 AM: Message edited by: plasttav ]

[Bolts-and-nuts]

AH OK, Customize drill cycle!!! that would be OK...

 

Thanks for all your help!!!

[Harryman]

Right on Iskander. I was just offering a little sample of what it might look like, not an entire routine.

 

Philippines to Kansas, killer commute Dude.

[Bolts-and-nuts]

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

Philippines to Kansas, killer commute Dude.

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

 

its a good way to save on labor!

 

isn't it?

[Rekd™]

quote:

---

This has been covered before and I believe that Rekd actually posted his format to be copied by anyone.

---

Yes, do it with a drill cycle. No edits. All via MC.

 

'Rekd

[MACHINEMASTERG]

we do this with a subroutine at the begining of the program call a sub that has your stop pin program in it and edit the sub as needed works great for machines with out the macros

[F. JAVIER]

One more way would be to draw line going in the "z" vector to the depth you need your pin to be and from the bottom depth another line in the direction your pin needs to move out, (away from the mat'l) then contour that chain so that the plane mask is off; then you go to your contoured operation and under options use the editor and add the M00 after the pin goes to depth....

 

Yeah, yeah the drill way is a lot better, I don't have it set that way yet, just giving another option to get it there; I guess I should get off of my .... and start working on it.....

F. Javier