Post Retract end of G71 Canned Cycles?

[R_Hawk_one]

Hello all. After years of getting burned by our posts, I have finally got them down to posting near perfect code I just need one last thing, posting a retract to initial approach on a G71 Canned cycle. It would be stellar if I could get it to post this on an ID turning cycle only. I'm not going to lie, I'm a COMPLETE NOOB and it's taken me about a week (working on them whenever I get "free time") but I'm comfortable editing the posts now as I have multiple backups as well. If anybody could point me in a decent direction it would be greatly appreciated. 

Posts are Generic MPL_HAAS and Generic Fanuc 4X MT_Lathe.

[crazy^millman]

Ref Points it is the best way to control this for Lathe.

[R_Hawk_one]

 

26 minutes ago, C^Millman said:

Ref Points it is the best way to control this for Lathe.

Thank you for the response, however for whatever reason on a canned cycle only the Ref Points are ignored and only at the END of the cycle.

This is what's posted:

G50 S1500
G96 T0606 S425 M03
G00 X1.625 Z.105 M08
G71 P30 Q40 U-.03 W.005 D.1 F.008
N30 G00 X3.6174
G01 Z-.0183
X3.5474 Z-.0533
Z-.475
N40 X1.625
M09
G00 G28 U0. W0.
T0600
M01

 

This is what I would like to have posted:

G50 S1500
G96 T0606 S425 M03
G00 X1.625 Z.105 M08
G71 P30 Q40 U-.03 W.005 D.1 F.008
N30 G00 X3.6174
G01 Z-.0183
X3.5474 Z-.0533
Z-.475
N40 X1.625
G00 Z.105 ( <~~~~ THIS )
M09
G00 G28 U0. W0.
T0600
M01

[mkd]

So what got messed up in the post to NOT output REF points? It's kinda a critical feature.

Being a self described NOOB, the experienced MC user would assume you are not use the REF points correctly, as its one of those "things" that'll burn new users.

[R_Hawk_one]

2 minutes ago, mkd said:

So what got messed up in the post to NOT output REF points? It's kinda a critical feature.

I'm not sure. AFAIK this is a stock, basic MCAM post that came with the software 100 years ago. The only thing I have to compare the post with is the Generic_Fanuc 4X MT_Lathe post that DOES output the code I need but that's an apple to orange comparison.

[crazy^millman]

Make a sample file and put it up here. This process should work if it doesn't it needs to be reported to QC.

[R_Hawk_one]

15 minutes ago, C^Millman said:

Make a sample file and put it up here. This process should work if it doesn't it needs to be reported to QC.

Are you looking for an actual MCAM file? 

[Guest]

1 minute ago, R_Hawk_one said:

Are you looking for an actual MCAM file? 

z2g so the post and machine & control defs come along

[R_Hawk_one]

30 minutes ago, JParis said:

z2g so the post and machine & control defs come along

 

cctest.ZIP

[mkd]

4 hours ago, R_Hawk_one said:

 

cctest.ZIP

mike,

your REF points under toolpath parameters are turned off.

 

[wdg5555]

I setup my lathes posts to go to Z1.0 at the beginning and end of every tool path. This works as long as your Z zero is always at the front of the part.  You could make a variable to  add 1" to the zabs variable if your Z zeros are not always at the front of the part. Only time I have to hand edit is when I use a tailstock, which is rare for me. And the best reason for doing it this way is you don't have to setup stock or reference points.

Below is the code I use, you will have to pull up the debugger most likely to figure out where exactly to put this in your post.

 

In section ltlchg$

"G0", pfxout, "Z1.0", e$

 

In section pl_retract$

"G0 Z1.0", e$

[Guest]

10 hours ago, wdg5555 said:

I setup my lathes posts to go to Z1.0 at the beginning and end of every tool path. This works as long as your Z zero is always at the front of the part.  You could make a variable to  add 1" to the zabs variable if your Z zeros are not always at the front of the part. Only time I have to hand edit is when I use a tailstock, which is rare for me. And the best reason for doing it this way is you don't have to setup stock or reference points.

Below is the code I use, you will have to pull up the debugger most likely to figure out where exactly to put this in your post.

 

In section ltlchg$

"G0", pfxout, "Z1.0", e$

 

In section pl_retract$

"G0 Z1.0", e$

I despise post edits like this....

I never like to hard code a position......the post at that point has NO idea where it is......

To each his own I suppose but not an edit I would make........

JM2C YMMV

[crazy^millman]

1 hour ago, JParis said:

I despise post edits like this....

I never like to hard code a position......the post at that point has NO idea where it is......

To each his own I suppose but not an edit I would make........

JM2C YMMV

Agreed why I said use ref points to begin with.

[R_Hawk_one]

12 minutes ago, C^Millman said:

Agreed why I said use ref points to begin with.

Has anybody tried using the Ref points? Because as I stated above^^^ it is ignored and it is not posted.

[crazy^millman]

8 minutes ago, R_Hawk_one said:

Has anybody tried using the Ref points? Because as I stated above^^^ it is ignored and it is not posted.

You are using a post from 2002 and you are expecting something that is made 15 years ago to be perfect? I would seriously consider updating to a 2017 post and see if the same thing happens. There were many changes to the output process that specifically addressed these types of issues with posts and by using a post this old I have to say that is the cause. You can spend weeks sorting out an old post or move to a new post and be done with it.

 

Here is posted code using REF points from the 2017 HAAS lathe post that ships with every seat of Mastercam. You will notice I get Z1.0 at the beginning and end of the G71 because I used Ref Points. I am not even going to try it with your post as I am sure it is broken.

%
O0000
(777)
(DATE=DD-MM-YY - 13-06-17 TIME=HH:MM - 06:23)
(MCX FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2017\MCX\CCTEST\USERS\MIKE FUSCO\DOCUMENTS\MY MCAM2017\MCX\MISC\CCTEST.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2017\LATHE\NC\777.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 6 OFFSET - 6)
(ROUGH ID PROFILE  INSERT - CCMT 3(2.5)2 UM 4015)
G28 U0. W0.
G50 X10. Z10.
T606
G97 S999 M03
G0 X1.625 Z1. M8
G50 S3600
G96 S425
Z.105
G71 U.1 R.025
G71 P10 Q20 U-.03 W.005 F.008
N10 G0 X3. S425
G1 Z-2.99
N20 X1.625
G0 Z.105
Z1.
M9
G28 U0. W0. M05
T600
M30
%

 

[R_Hawk_one]

1 minute ago, C^Millman said:

You are using a post from 2002 and you are expecting something that is made 15 years ago to be perfect? I would seriously consider updating to a 2017 post and see if the same thing happens. There were many changes to the output process that specifically addressed these types of issues with posts and by using a post this old I have to say that is the cause. You can spend weeks sorting out an old post or move to a new post and be done with it.

 

Here is posted code using REF points from the 2017 HAAS lathe post that ships with every seat of Mastercam. You will notice I get Z1.0 at the beginning and end of the G71 because I used Ref Points. I am not even going to try it with your post as I am sure it is broken.

%
O0000
(777)
(DATE=DD-MM-YY - 13-06-17 TIME=HH:MM - 06:23)
(MCX FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2017\MCX\CCTEST\USERS\MIKE FUSCO\DOCUMENTS\MY MCAM2017\MCX\MISC\CCTEST.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAM2017\LATHE\NC\777.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 6 OFFSET - 6)
(ROUGH ID PROFILE  INSERT - CCMT 3(2.5)2 UM 4015)
G28 U0. W0.
G50 X10. Z10.
T606
G97 S999 M03
G0 X1.625 Z1. M8
G50 S3600
G96 S425
Z.105
G71 U.1 R.025
G71 P10 Q20 U-.03 W.005 F.008
N10 G0 X3. S425
G1 Z-2.99
N20 X1.625
G0 Z.105
Z1.
M9
G28 U0. W0. M05
T600
M30
%

 

Um, I don't recall saying I expected the posts to be perfect. I was completely unaware new posts came with the new software as I wasn't told about it at the seminar or by our re-seller. Add to that the 2002 post is actually closer to what I needed save for not posting DOC and pulloff values and it would probably have taken me longer to edit the post you referenced than the 2002 post anyways.

I kind of inherited a little bit of a mess without much to go on and as we all know full well re-sellers are rather not so helpful and the first thing they do is hold out their hand looking for bills. Thanks, I think.

[Guest]

10 minutes ago, R_Hawk_one said:

as we all know full well re-sellers are rather not so helpful and the first thing they do is hold out their hand looking for bills.

Really?

I worked for a reseller for 6+ years.....did hundreds of quick little post edits with zero charge....

I'm guessing Opti-Pro is your reseller, I know Chris and Vince might want to give them a chance

[crazy^millman]

1 minute ago, R_Hawk_one said:

Um, I don't recall saying I expected the posts to be perfect. I was completely unaware new posts came with the new software as I wasn't told about it at the seminar or by our re-seller. Add to that the 2002 post is actually closer to what I needed save for not posting DOC and pulloff values and it would probably have taken me longer to edit the post you referenced than the 2002 post anyways.

I kind of inherited a little bit of a mess without much to go on and as we all know full well re-sellers are rather not so helpful and the first thing they do is hold out their hand looking for bills. Thanks, I think.

I wasn't told posts came with the software either. I went into the directory where posts are stored on the machine and found it. I don't know your situation and not going to get into a conversation about you and your dealer. You do want your post to work perfect if you don't then why are you even asking a question? We all want our post to work perfect if they don't then why have one? Sorry I have programmed Mastercam lathe for many years and was trying to point you in the right direction with ref points. I am very busy and do my best to help people on here and seen the zip file and thought okay cool someone will help you. They said you didn't have ref points on in the file. I have to assume you didn't either when you tried it. Again no disrespect, but if I want someone to help me with a specific problem I show them the specific problem I am having by sending a file with ref points turned on. By not having them on you leave the door open for someone to think you were not using them. We are not sitting next to you we are not doing a gotomeeting seeing what you are seeing so cut us some slack as we do this to be a blessing to others. I am no one special, but my experience tells me if I don't see the problem the exact way someone tells me it is then I have to ask are they doing it correctly.

You want that posts to do what you need then look at the newer post and do a file compare and see what the differences are. Run a debugger on both and see why the new one works and the old one doesn't. After you spent all the time you tell me which way is the better way. Minor adjustments to a newer post that support the current software or a post that you hope will keep supporting the modern software?

I am sure someone will read this and tell me how mean and ugly I am being and that is not my intent here, but how about seeing the other side of the equation not just from your seat how about maybe from my seat. 

 

[R_Hawk_one]

49 minutes ago, JParis said:

Really?

I worked for a reseller for 6+ years.....did hundreds of quick little post edits with zero charge....

I'm guessing Opti-Pro is your reseller, I know Chris and Vince might want to give them a chance

Yes, Opti-Pro is our re-seller. They have been good to us, I'm not trying to imply they aren't but they (rightfully so) wanted money for a post for a brand new multi-axis lathe nobody else bought yet that we purchased about a year ago therefore I had no choice but 1- Hand edit a LOT of code for every program, 2-Fight with management until they forked over the cash for a post 3-Edit the post myself. I decided to edit the post myself and have got it down pretty good.

So I fixed the posts for our other machines myself as well and up to this point every one of those other machines posts perfect code EXCEPT this retract issue, so I hopped on here to see if maybe somebody else might have dealt with this issue and here we are LOL.

49 minutes ago, C^Millman said:

I wasn't told posts came with the software either. I went into the directory where posts are stored on the machine and found it. I don't know your situation and not going to get into a conversation about you and your dealer. You do want your post to work perfect if you don't then why are you even asking a question? We all want our post to work perfect if they don't then why have one? Sorry I have programmed Mastercam lathe for many years and was trying to point you in the right direction with ref points. I am very busy and do my best to help people on here and seen the zip file and thought okay cool someone will help you. They said you didn't have ref points on in the file. I have to assume you didn't either when you tried it. Again no disrespect, but if I want someone to help me with a specific problem I show them the specific problem I am having by sending a file with ref points turned on. By not having them on you leave the door open for someone to think you were not using them. We are not sitting next to you we are not doing a gotomeeting seeing what you are seeing so cut us some slack as we do this to be a blessing to others. I am no one special, but my experience tells me if I don't see the problem the exact way someone tells me it is then I have to ask are they doing it correctly.

You want that posts to do what you need then look at the newer post and do a file compare and see what the differences are. Run a debugger on both and see why the new one works and the old one doesn't. After you spent all the time you tell me which way is the better way. Minor adjustments to a newer post that support the current software or a post that you hope will keep supporting the modern software?

I am sure someone will read this and tell me how mean and ugly I am being and that is not my intent here, but how about seeing the other side of the equation not just from your seat how about maybe from my seat. 

 

I didn't get on here to start pissing matches or to waste anybody's time. I specifically left out turning Ref points on because I didn't want someone to open up the file and think maybe it was jut a glitch or something as I had stated previously even when turning them on it's ignored. I was just hoping somebody on here had dealt with this issue and knew where it might be in the post. That's all.

[wdg5555]

4 hours ago, JParis said:

I despise post edits like this....

I never like to hard code a position......the post at that point has NO idea where it is......

To each his own I suppose but not an edit I would make........

JM2C YMMV

I knew my suggestion would not go over well

But this avoids having to setup stock. The little bit I have used stock it is a pain to use. And even if its not a pain to use its still an unnecessary /extra step to do. Additionally what happens if you program a boring bar and you forgot to setup your stock or your reference points? CRASH! My post edit is foolproof, which the less I have to use my brain the better my day seems to go.

[Guest]

6 minutes ago, wdg5555 said:

My post edit is foolproof,

Until they make a smarter fool....

Running lathe without stock defined, listen, it works for you great.....but stock should be defined as the very first thing a user does in lathe....

IMO, it's just lazy no to do so...

 

Now R_Hawk_one....

Your post just isn;t equipped to handle the reference points....I tried it in the base version of the MPLFAN and it posted fine.

Post processors DO have a shelf life....my opinion, this post has reached it...  the edits aren't huge, I would really suggest it be time for a new post

[mkd]

26 minutes ago, wdg5555 said:

I knew my suggestion would not go over well

But this avoids having to setup stock. The little bit I have used stock it is a pain to use. And even if its not a pain to use its still an unnecessary /extra step to do. Additionally what happens if you program a boring bar and you forgot to setup your stock or your reference points? CRASH! My post edit is foolproof, which the less I have to use my brain the better my day seems to go.

it's not a MC bug, it's a feature

this has been around a long time in lathe. Not sure of the the fixes over the years but a more robust detection system would have been appreciated when i was new. Kinda funny having a cam system that'll so easily send a boring bar home in X while still in the bore. Can't think of a time when this should EVER happen on purpose. Flame suit on. :-(

 

[R_Hawk_one]

1 hour ago, JParis said:

Until they make a smarter fool....

Running lathe without stock defined, listen, it works for you great.....but stock should be defined as the very first thing a user does in lathe....

IMO, it's just lazy no to do so...

 

Now R_Hawk_one....

Your post just isn;t equipped to handle the reference points....I tried it in the base version of the MPLFAN and it posted fine.

Post processors DO have a shelf life....my opinion, this post has reached it...  the edits aren't huge, I would really suggest it be time for a new post

I guess I'm just going to have to modify a newer version in my spare time. Thanks for the insight, appreciate it.

[Guest]

8 minutes ago, R_Hawk_one said:

I guess I'm just going to have to modify a newer version in my spare time. Thanks for the insight, appreciate it.

Short term, I know it seems like a PITA....long term, I think you'll find yourself happier and more equipped to handle different situations

 

[crazy^millman]

11 minutes ago, R_Hawk_one said:

I guess I'm just going to have to modify a newer version in my spare time. Thanks for the insight, appreciate it.

Post the code with the new post and then post with the old. Show us the difference and we will be glad to help you get it taken care of.