drill long format

[Robby GM]

we use long ouput for our drill operations

just noticed not getting same amount of peck

in nc file that we put in peck amount box

input 5 mm and nc has 2mm picks

tryed changing pick %dia, no change

we do not use materal list...

any ideas as to were to look next..

 

ps: ver 8.1.1 and using MPmaster post

 

[ 12-03-2002, 10:44 AM: Message edited by: Robby GM ]

[Surface]

There exists a "first peck" and "subsequent peck" dialog box. Is it possible that the "subsequent peck" box is fighting you?

[Robby GM]

subsequent peck dialog box is grayed out

post has peck1 only in it

[cadcam]

Robby waht is the control and what post are you using?

[Robby GM]

controls are cincinnati 850sx

post is Mpmaster post

[Roger Martin from CNC Software]

quote:

---

There exists a "first peck" and "subsequent peck" dialog box. Is it possible that the "subsequent peck" box is fighting you?

---

Quite right !

 

If you have the post setup for long-hand output for Peck drilling, the values shown for ->

 

Subsequent peck and Peck clearance

 

ARE going to be used (does not matter that they are 'greyed out'. The TXT file for the post you are using is doing the 'gray out' on those input boxes.

 

To enable those fields you need to alter the TXT file.

 

 

*** Is this in the v8 MPMASTER.TXT ->>

 

[peck drill]

1. "G83 - Peck Drill"

2. "Feed rate"

3. "Dwell"

4. "Clearance..."

5. "Retract..."

6. "Depth..."

7. "1st peck"

8. ""

9. ""

10. ""

11. ""

 

*** CHANGE to this ->>

 

[peck drill]

1. "Peck Drill"

2. "Feed rate"

3. "Dwell"

4. "Clearance..."

5. "Retract..."

6. "Depth..."

7. "1st peck"

8. "Subsequent peck"

9. "Peck clearance"

10. ""

11. ""

 

After altering the TXT fkle for a post you MUST either;

Re-start Mastercam

or

Change to a different post processor and then change back to your post.

[cadcam]

Thanks Roger I was figureing that one of you from CNC or Inhouse would show with the answer to fix the post.

[Robby GM]

ill try it at work weds and let u know

thanks all

[Christian Raebild]

The text file will also be updated if you select NC Utils -> Post process -> Change, and then select the existing post processor.

[Robby GM]

Thank You Roger

that did it.

[Roger Martin from CNC Software]

quote:

---

The text file will also be updated if you select NC Utils -> Post process -> Change, and then select the existing post processor.

---

* Note for anyone reading this thread. *

 

This solution will NOT work for what Robby needed. The UpDatePST utility will update the .TXT file to work with Mastercam v9, but would NOT alter the text that appears on the canned cycle parameters page!

[Allan Brown]

I think Christian is saying that you don't need to shut down Mastercam or change to a different post to refresh the menu text based on the post's txt file - you just need to 'change' to the post you are already running in order to cause the refresh.