Canned cycle doesn't post first hole location

[Kduhn66]

I'm not sure how or when it happened but the post I've been using decided to start not posting the first hole location when doing canned hole cycle. It's on a haas machine with generic haas post.

This is what it should look like

N130 G0 G90 G54 X-18.25 Y7.75  S5000 M3N140 G43 H5 Z2.N150 M8N160 Z.1N170 G99 G81 X-18.25 Y7.75 Z-.25 R.1 F50.N180 Y7.125

Thats what it post

N130 G0 G90 G54 X-18.25 Y7.75 S5000 M3

N140 G43 H5 Z2.N150 M8N160 Z.1N170 G99 G81 Z-.25 R.1 F50. --------no hole locationN180 Y7.125

This is how it post it- causing it to skip the first location and go to the second, Y7.125 in this case.

Is there either a fix to this or can someone point me where to find an original Haas post- our reseller isn't of much use, you have to pay them about 400$ and hour just to stand outside their office and look at it.

[Radical1]

This post may look like it won't work, but in reality it will still drill the first hole location because the fixed cycle will start at the present location. The X Y location you have in the fixed cycle call is optional in most, if not all machine controls.

[Kduhn66]

It skips it- I've tried already, i had to manually put in first location on the G81 line

[landscnc]

Every HAAS I run if thers no L0 on G81 line it will drill where it sits then start locations after G81 line is there a setting in control I can't remember that and I'm home not work

[landscnc]

Oh yeah and we don't put X Y Location on G81 line either just the way we manually program for years

[crazy^millman]

I'm not sure how or when it happened but the post I've been using decided to start not posting the first hole location when doing canned hole cycle. It's on a haas machine with generic haas post.

This is what it should look like

N130 G0 G90 G54 X-18.25 Y7.75  S5000 M3N140 G43 H5 Z2.N150 M8N160 Z.1N170 G99 G81 X-18.25 Y7.75 Z-.25 R.1 F50.N180 Y7.125

Thats what it post

N130 G0 G90 G54 X-18.25 Y7.75 S5000 M3

N140 G43 H5 Z2.N150 M8N160 Z.1N170 G99 G81 Z-.25 R.1 F50. --------no hole locationN180 Y7.125

This is how it post it- causing it to skip the first location and go to the second, Y7.125 in this case.

Is there either a fix to this or can someone point me where to find an original Haas post- our reseller isn't of much use, you have to pay them about 400$ and hour just to stand outside their office and look at it.

 

Funny you say that and I go back to many of the dealers I personally work with and it is the companies that never want to pay for anything. They are normally the ones that come complaining about their dealers. We get your side of the story, but not theirs so if you go into the post in the drill cycle and put a * in front of the X and Y output variables you will get the X and Y output in the first line of the drilling code in the post. Any very jr wet behind the ears AE knows this. 

 

I am going to go out on a limb an susepct you have not the first clue what I am talking about. Here you go something someone who really wants to learn does. They do a search on the forum and find the following topics about drilling cycles for posts in Mastercam.

http://www.emastercam.com/board/topic/77548-is-there-away-i-can-have-any-idea-how-to-use-g1213/?p=921842

 

BTW Welcome to the forum and everyone considers me the mean one around here. I have this issue with just telling things like they are.

[Kduhn66]

we actually Pay for a yearly maintenance fee. So I think they should help us out right? It's not so much that they want to charge for everything, little sarcasm- its trying to get a hold of them and them email or calling back. I haven't done anything with the actual post in a long time (and even that was minimal) and i'm not about to start guessing and mess it up. I'll look for the canned variables and add the *

It's still odd that it just started doing it though still.

 

Weird that it skips for us. There may be a setting but I don't think any operators would change it.

[crazy^millman]

we actually Pay for a yearly maintenance fee. So I think they should help us out right? It's not so much that they want to charge for everything, little sarcasm- its trying to get a hold of them and them email or calling back. I haven't done anything with the actual post in a long time (and even that was minimal) and i'm not about to start guessing and mess it up. I'll look for the canned variables and add the *

It's still odd that it just started doing it though still.

 

Weird that it skips for us. There may be a setting but I don't think any operators would change it.

 

Well here is where you want to look in the post:

pdrill$          #Canned Drill Cycle
      pdrlcommonb
      pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout,
        prdrlout, dwell$, *feed, strcantext, e$
      pcom_movea

If a 3 axis machine then the pxout and pyout will be where you want to add the * in front of. Most modern posts have a pfxout and pfyout that does the same thing, but the * is the easiest choice to do for a rookie post person. If the Z changes then it will output the changes, but 99.99% of the time the 1st hole should be the same depth as the cycle has called out. I would not recommending adding the * in front of the Z unless your machine is still freaking out.

 

Funny how people bash the dealers yet most times never really have talked to them. I have dealt with many of the Mastercam dealers national and international and I have found almost everyone to be very responsive and have great relationships with customers. Yet many come in here like I did when I 1st started coming on this forum and complaining without really taking the time to reach out the dealer and see if they really can help them out or not. Sorry not meant to beat you up about this, but we(the average emastercam user) are here to help not listen to complaints about your dealer. Got a problem with your dealer email CNC Software the makers of Mastercam other than that come in here and ask for help and wade through the mud so to speak making effort and most people will respond to help you out. Come in here bashing and trashing talking why would anyone want to help? Next thing you know that person helping you will be getting the same treatment. Hopefully this is some food for thought for those that seem to think doing this type of behavior really gets them anywhere because guess what it doesn't.

[AlbertZini]

pdrill$ #Canned Drill Cycle

pdrlcommonb

pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,

prdrlout, dwell$, *feed, strcantext, e$

pbld, n$, pfxout, pfyout, e$ # <------------

pcom_movea

 

[crazy^millman]

pdrill$ #Canned Drill Cycle
pdrlcommonb
pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,
prdrlout, dwell$, *feed, strcantext, e$
pbld, n$, pfxout, pfyout, e$ # <------------       
pcom_movea

 

 

Albert sorry I am going to say that is a bad approach to this problem. If the point changes when doing different locations then you would get a duplicate output of the same place?

[Guest]

I'm not sure how or when it happened but the post I've been using decided to start not posting the first hole location when doing canned hole cycle. It's on a haas machine with generic haas post.

This is what it should look like

N130 G0 G90 G54 X-18.25 Y7.75  S5000 M3N140 G43 H5 Z2.N150 M8N160 Z.1N170 G99 G81 X-18.25 Y7.75 Z-.25 R.1 F50.N180 Y7.125

Thats what it post

N130 G0 G90 G54 X-18.25 Y7.75 S5000 M3

N140 G43 H5 Z2.N150 M8N160 Z.1N170 G99 G81 Z-.25 R.1 F50. --------no hole locationN180 Y7.125

This is how it post it- causing it to skip the first location and go to the second, Y7.125 in this case.

Is there either a fix to this or can someone point me where to find an original Haas post- our reseller isn't of much use, you have to pay them about 400$ and hour just to stand outside their office and look at it.

 

If all you need is the drill points to come out on the G81 line just force the output

 

Change this

pdrill$          #Canned Drill Cycle
      pdrlcommonb
      pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,
        prdrlout, dwell$, *feed, strcantext, e$
      pcom_movea

to this

pdrill$          #Canned Drill Cycle
      pdrlcommonb
      pcan1, pbld, n$, *sgdrlref, *sgdrill, pfxout, pfyout, pfzout, pcout,
        prdrlout, dwell$, *feed, strcantext, e$
      pcom_movea

If you really need that position output on those lines, you may have to edit your other cycles as well

 

 

Also, is this an MPMaster post processor? You say it suddenly stopped outputting the position is it possible this this got turned off?

 

force_dpts  : no$   #Force XY output on all drilling lines including cycle call?

[Kduhn66]

Adding the F did the trick- the * didn't seem to work. I did finally hear back from our dealer so that was nice- he confirmed the same thing with adding the F. 

And Ron one of the reasons we have had problems with our dealer is at one point they were bought out, moved locations and then didn't inform people. we had to hunt them down. That's frustrating. maybe after switching to a new owner they are better.