Tool Name in post

[machtek]

Hi all, New job new post problems. Is there any way to post with the tool name after the dia?

 

This is what I want:

code:

---

 (TOOL  T1 =6.45 DIA. FACE MILL)

(-------------------------------)

 

G90 G0 G54 X19.225 Y-7.775

G43 H1 Z2. M08

S2000 M3

Z.5

---

This is what I get:

code:

---

 (TOOL  T1 =6.45 DIA.)

(-------------------------------)

 

G90 G0 G54 X19.225 Y-7.775

G43 H1 Z2. M08

S2000 M3

Z.5$

---

Thanks if advance

[crazy^millman]

Look to the Mpmaster Post offered on this web site I think you will be very happy you did.

 

HTH

[machtek]

you're right, I am very happy I did. Now what do I do with it to help solve the problem. At this point you must realize I am almost totally ignorant in the ways of modifying posts.

 

Thanks

[Kannon]

after selecting the different post processor are you still not getting the comment?

[machtek]

I do get the tool name output however the other stuff that makes the old post work for that machine is gone. I hate to start all over again and would like to modify the old post to include the tool name.

[Kannon]

looks like your missing something in your ptoolcomment. Compare the ptoolcomment between the 2 Post processors.

 

code:

---

ptoolcomment  #Comment for tool

tnote = t

toffnote = tloffno

tlngnote = tlngno

"(", pstrtool, *tnote, *toffnote, *tlngnote, *tldia, ")", e

 

pstrtool #Comment for tool

if strtool <> sblank, pstrtool2

 

pstrtool2 #Comment for tool

strtool = ucase(strtool)

*strtool, " "

---

[machtek]

There is something missing, the whole tool comment section. No wonder it doesn't work. Looks like I better learn at least the first thing about modifying posts. We are currently hand writing the tool comment and it gets old after one of two program changes.

[crazy^millman]

Well I would contact your dealer and tell them what you are looking for and see what it would take for them to do it for you.

 

Here is from MPMASTER untouched:

 

code:

---

%

O4343 (M94343)

N100 M00

N110 (REMOVE 2 CLAMPS ON TABS)

(DATE - MAR-12-2007)

(TIME - 5:14 AM)

(T2 - 1 INCH ENDMILL - H2 - D2 - D1.0000")

(T12 - 3/4 BULL ENDMILL 0.125 RAD - H0 - D0 - D0.7500" - R0.1250")

(T15 - 1-1/4 FLAT ENDMILL - H15 - D15 - D1.2500")

(T1 - 1/4 CENTERDRILL - H1 - D0 - D0.2500")

(T21 - NO. 3 DRILL - H21 - D0 - D0.2130")

(T22 - NO. 1 REAMER - H22 - D0 - D0.2280")

(T23 - 15/64 DRILL - H23 - D0 - D0.2344")

(T24 - 1/4 REAMER - H24 - D0 - D0.2500")

(OVERALL MAX - Z6.)

(OVERALL MIN - Z-.1704)

N120 G0 G17 G20 G40 G80 G90

N130 T2 M06 ( 1 INCH ENDMILL)

N140 (MAX - Z6.)

N150 (MIN - Z-.01)

---

[machtek]

That may be the wise choice. Thanks for all the advice!

[Mr. Dayshift]

Machtek, use SEARCH. I found it using 'tool comment'. I don't recommend it.

 

I think it's easier is to right click on your operations window, select set up sheet, and click on box with tool graphics and numbers. When that document opens, you can print it.

 

I am assuming you are not running the machine.

[machtek]

been there done that Curt. It doesn't exist. This post if from 92, thats right 1992

[Guest]

quote:

---

This post if from 92, thats right 1992

---

Time to retire it meh thinks.

[machtek]

You are very right. Will the company go for it, they been around for 38+ years and I can hear it already. It's been working up to now! I am only on my 4th day here. I have a hard time though understanding why a programer will open a posted program and spend time "fat fingering" it when the post is what needs the attention. Like I said, I better learn at least the first thing about modifying one.

[Colin Gilchrist]

Machtek,

 

What machine is is for? Most machines require very little modification for MPMaster to work right. If you let us know what type of Machine and Control you have, and what changes you need to make to MPMaster, we can help you get it up and running. You'll also learn more than you wanted to about Posts.

[crazy^millman]

Now if this is for your 5 axis machines then Mpmaster will not work. However you can take parts of MpMaster and integrate them into any post. I have done it does require some work, but is easily done.

 

HTH

[cobra95kev]

Machtek,

I feel your pain. When I came to this job 3 months ago I had never ran mastercam at all.

(only Gibbs)

So I came in my first day never having seen MCAM and they have 9 and 10 here. Well the guy before me had quit before I got here and he had never even touched 10. So I decide there was no reason for me to learn 9 since it was outdated so to make a long story short I had to learn MCAM 10 and at the same time learn how to update posts from ver9 (which usually didn't work to well) and learn how to modify posts too.

 

I wouldn't have been able to do any of it without all of the help from people like John P. and some others who have helped through E-mail.

 

This is a great community. I just wish I knew enough to be of more asistance. With time I guess.

 

Later,

Kevin C.

[doyleg]

why can't he just copy what Kannon has in his post and insert it into his. He only has to insert it before or after 'start of file and tool change set-up. and then put "ptoolcomment" in to the correct place in the post? are there more things involved with this comment or is it that simple.

[machtek]

cobra95kev, I feel you, eight years in gibbscam (and virtual gibbs) then on to 9.1 then x then mr1-mr2 now back to 9.1, wtf. All in a days work, the man wants a green suit turn on the green light right?

 

doyleg, this is about what I was thinking, John or Ron or Kannon, do you know where this could be dropped into the post I have so I can get the benefits without getting too much attention?

 

again thanks all

[doyleg]

In mine, a variation of what Kannon has is before the 'start of file and tool change set-up'. then at the tool change it has - ptoolcomment, - after the "m6" at the tool change line but before the e$ .

[Guest]

quote:

---

why can't he just copy what Kannon has in his post and insert it into his.

---

Because, he needs to define ALL of the variables, many of the tool lists are created by a call at the start of the post, the pwrtt section. I don't know if this "old" post will even have the call.

 

There is no reason what so ever NOT to update, especially if this is a 3 or 4 axis mill.

 

It will likely take less time to get the new MPMaster up and running than it will tweaking around trying to get the old one just so you'd like it.

 

JM2C

[machtek]

I have your point John. Like I said, I will endeavor to learn the first thing about post mods. The posts arent really that different from one another but under fire we don't have a lot of time for learning. The very reason for subscribing to this forum. Many great ladies and gentlemen here and hundreds if not thousands of years of combined experience. I will identify what anomolies mpmaster is outputting and try to ask a few focused questions in the very near future.

 

Again Thanks

[Guest]

machtek, I don't know if you can do this or not but when I first starting digging into posts I did it on my own time. Took the SIM home and did it there. Then when the post was "ready" I would just start using it. I, of course, would pay very close attention to the code for awhile.

 

Now, there are fews edits that I can't make within just a few minutes. If I have a big or new one to work out, I still do it at home.

[machtek]

John, that's pretty much what I had in mind. Better to learn when not under fire, the wife will just have to entertain herself for a while!

[Bryan Johnson]

the variable for tool name is "strtool".

 

before:

"(TOOL ", t, "=", tldia, "DIA.)"

 

after:

"(TOOL ", t, "=", tldia, "DIA.", strtool, ")"

 

you may also need to add this line to your "General output settings"

strtool_v7 : 2 #Use Version 7+ toolname?

 

but check that it is not already there 1st.

 

send me a copy of the post, and I can modify it for you. I need to move you guys to X.

[machtek]

Thanks Bryan, that did the trick.

 

We have X, the problem is that when a former programer left, his stuff was in X and the old timer here struggled and eventually had to rewrite many of the X programs back to 9. Just by necessity, he hasn't picked up x with the needed speed due to work load. He has mentioned the desire to move forward but I can witness that he doesn't have time currently.