g54 surprises

[JHintze]

very newbie topic i believe. so im getting random g54s posting in my programs. it doesnt always happen on every tool in a toolpath group. im aiming to have NC files post with no work offsets in them at all, we leave it to the operators to place the correct offsets in the programs or in the mains.  

 

question 1 is why does it post sometimes and not always on me? it usually isnt the whole program or even a whole toolpath group. today i had it post only in one toolpath group and only on 90% of the tools in that group.

 

question 2 i have found that under a toolpaths parameter under misc values if i check the box labeled "Automatically set to post values when posting"(see attached file)  it removes the offset from posting, will the cause any other unseen surprises after posting? and how can i avoid not having to check this box everytime?

 

[crazy^millman]

Newbie question? Sorry, but that is just an overall bad practice. You always put workoffsets in a CNC program sent to floor always. I have never worked in a shop or run a shop where sending the program to the floor did not have a workoffset. I was the Shop Foreman in one shop where we had over 70 CNC machines and we never sent or allowed programs to be at the discretion of the operators. They are allowed to change workoffets, but it is a better practice to do a mass edit of work offsets verses adding them. What if they miss something who is responsible? I see a lot of finger pointing going on at your shop, disorder and just havoc at the best.

 

Sorry if my response seems rough, but I have personally been in well over 200 different shops programming projects and never heard of such a thing. I do my best to give honest and accurate methods for programming CNC Machines. This process is not a good practice and not one I can give you an answer on how to resolve since it goes so far against the very fabric of sound practices I wouldn't want anyone to adopt this concept, idea or direction. Please reconsider and have a shop meeting to resolve and head this in a better direction for you and your company's well being.

 

Last night heading on my way home from church there was a person in the middle of the road. He was trying to cross a 6 lane road and walked into a car. The person who's car he hit was standing the middle of the road trying to stop cars. I immediately stopped put my flashers on stopped the cars behind me. Once I saw the cars were respecting what was going on I came to there aid. Point is I just do what I think it right and might have saved a life last night. Make me no one special, but how many cars(people) would have not paid attention and hit him or the other vehicle? I see something that is a major issue here and not trying to beat up on anyone just the person I am doing my best to help others.

[gcode]

open your post and make sure this line is set to yes

 

force_wcs   : yes$  #Force WCS output at every toolchange?

 

then set  the Misc inter 9 "Lock on first WCS" to 1

Then  you should get G54 in all ops

 

you could try opening your post and changing this line to 3

 

wcstype     : 2     #0 = G92 at start, 1 = G92 at toolchanges, 2 = G54, 3 = Off

 

I've never tried this and as Ron said above, it's very dangerous...

sooner or later it will bit you ... hard

[JHintze]

thank you gcode for offering some kind of help, but i dont think its post related as it didnt happen to the last programmer that worked here.

 

i understand pushing good practice, but were in a unique situation. i work for a small shop with three machinists, me being one, running six mills and 2 lathes. I myself am very new to this industry and extremely new to programming. we do not use g54, g55 ect.. we use p1-p48. we rarely run the same part in a massive order. so we leave it up to the machinists as to where the part will be placed as of offsets. as we use mains to control what offset is going to what program, and anytime a g54 gets posted randomly into the program is where we have things getting smashed.

 

so let me rephrase my question :

 

my mastercam x9 randomly places offsets to random tools, its not post related as it didnt happen to the last programmer we had, but g54 gets posted to some tools but not all, and sometimes even g55 or g56 gets posted also. what settings control offsets within mastercam?

[gcode]

try opening you post

find this line

 

wcstype : 2 #0 = G92 at start, 1 = G92 at toolchanges, 2 = G54, 3 = Off

 

and change it the 2 to a 3

 

I've never tried this and have no idea if it will work

[jaydenn]

Take a look at your Plane Manager.

Have you set the offset or did you leave it default? I always set every plane because, as you've learned, Mastercam is unpredictable at best.

 

just type in "1" on every plane that's in use and you'll get g54 every time.

 

New Bitmap Image.bmp

[Guest]

Take a look at your Plane Manager.

Have you set the offset or did you leave it default? I always set every plane because, as you've learned, Mastercam is unpredictable at best.

 

just type in "1" on every plane that's in use and you'll get g54 every time.

 

New Bitmap Image.bmp

 

Incorrect type 0

 

0=G54

1=G55

2=G56

3=G57

4=G58

5=G59

6=G54.1P1

 

-1 = USE NEXT AVAILABLE OFFSET

 

If you're getting different outputs, you have different planes in use, each plane, unless locked down will create a new work offset output, that is how Mastercam functions.

 

Some basic training would teach you this

 

Jaydenn, if you're getting a G54 with a 1, your post has been edited to do that

[JHintze]

Incorrect type 0

 

0=G54

1=G55

2=G56

3=G57

4=G58

5=G59

6=G54.1P1

 

-1 = USE NEXT AVAILABLE OFFSET

 

If you're getting different outputs, you have different planes in use, each plane, unless locked down will create a new work offset output, that is how Mastercam functions.

 

Some basic training would teach you this

 

Jaydenn, if you're getting a G54 with a 1, your post has been edited to do that

 

thank you Jparis i think this is what i was looking for.

[jlw™]

Judging by the screenshot I'm guessing Misc Int #1 is the answer to the riddle.

[jaydenn]

Incorrect type 0

 

Jaydenn, if you're getting a G54 with a 1, your post has been edited to do that

You're right.

I generally make my posts "G53 + offset" cause that's just how I roll!

 

J

[htm01]

Incorrect type 0

 

0=G54

1=G55

2=G56

3=G57

4=G58

5=G59

6=G54.1P1

 

-1 = USE NEXT AVAILABLE OFFSET

 

If you're getting different outputs, you have different planes in use, each plane, unless locked down will create a new work offset output, that is how Mastercam functions.

 

Some basic training would teach you this

 

Jaydenn, if you're getting a G54 with a 1, your post has been edited to do that

you can take the teacher out of the classroom but you can't take the teacher out of JP

[Guest]

you can take the teacher out of the classroom but you can't take the teacher out of JP

 

No, sometimes not  

[htm01]

I think you miss it sometimes

[Guest]

I think you miss it sometimes

 

It had it's moments  

 

In all likelihood, if S4A had not been sold, I would likely still be there

[Newbeeee™]

I would seriously look at a bit of training and also look into a post mod so you can enter what you want in mcam and get output what you want for the machine.

And even output M00 as a possibility on every offset call, so the machine won't proceed. I don't know what you're doing, but there must be a better way of automating and making it failsafe.

It is an accident waiting to happen...

[JHintze]

I would seriously look at a bit of training and also look into a post mod so you can enter what you want in mcam and get output what you want for the machine.

And even output M00 as a possibility on every offset call, so the machine won't proceed. I don't know what you're doing, but there must be a better way of automating and making it failsafe.

It is an accident waiting to happen...

 

 

i really like the idea of a post mod that outputs a M00 if its also posting an offset. that would stop a lot rare crashing.

[Guest]

i really like the idea of a post mod that outputs a M00 if its also posting an offset. that would stop a lot rare crashing.

Actually, having a better idea of knowing what you're doing would go along way to not crashing...

 

Don't look to the post to fix programming bad habits

 

If you ever go some where else, your bad habits will follow but the post edits will not

[crazy^millman]

i really like the idea of a post mod that outputs a M00 if its also posting an offset. that would stop a lot rare crashing.

 

Easily done. Need to add this to your post. This is from the MPMASTER post. May look different so adjust to your post. Also all posts edits are use at your own risk.

pwcs            #G54+ coordinate setting at toolchange
      if wcstype = two | wcstype > three,
        [
        sav_frc_wcs = force_wcs
        if sub_level$ > zero, force_wcs = zero
        if sav_mi9 = 1, workofs$ = sav_workofs
        if workofs$ < 0, workofs$ = 0
        if workofs$ <> prv_workofs$ | (force_wcs & toolchng) | sof,
          [
          if workofs$ < 6,
            [
            g_wcs = workofs$ + 54
            *g_wcs, "M00" (WORKOFFSET ADDED)
            ]
          else,
            [
            if haas,
              [
              p_wcs = workofs$ - five        #G154 P1 to P99
              "G154", *p_wcs
              #g_wcs = workofs$ + 104        #G110 to G129
              #*g_wcs  
              ]
            if yasnac,
              [
              spaces$=0
              j_wcs = workofs$ - five        #G54 J1 to J99
              "G54", *j_wcs , "M00" (WORKOFFSET ADDED)
              spaces$=sav_spc  
              ]   
            else,
              [
              p_wcs = workofs$ - five
              "G54.1", *p_wcs, "M00 (WORKOFFSET ADDED)
              ]
            ]
          ]
        force_wcs = sav_frc_wcs
        !workofs$
        ]

This was not tested, but I think should do what was suggested.

 

Again I have been a Machinist for over 30 years and programmed CNC machines since High school back in the late 80's you are not going about this in a good method and are setting yourself up to fail. You are determined I give you that, but building good method and processes will aid you moving forward. Best of luck and hope don't tear something up or worse yet hurt someone.

[Matthew Hajicek - Singularity]

I used to work there.  What they have going on is that they'll run the same program on multiple offsets on different faces of a tombstone, two stations on each of four sides.  Usually there's a part A and a part B on each face of the tombstone, though sometimes a face or two may have parts C and D depending on what customers have ordered.  Then there's the other pallet which may have the same or a totally different set of parts.  The main sets the work offset and then calls the appropriate posted code as a sub, so the posted code needs to be free of work offsets.  The posted code also stays on file for reuse in future batches which will need different offsets.

 

How do other shops handle this type of situation?

[jlw™]

Macros.

 

I'll see if I can find some I used to use. I haven't had to mess with tombstones in 4 or 5 years. I had probe routines that identified and checked pallet/tombstone.

[Newbeeee™]

Thinking out loud, any advantage in assigning a M# against a 9000 or other background prog (Parameter 6072 etc)?

 

So

M54 can be G54

M55 G55

M56 G56 etc

 

Then have a main prog which when runs, has

 

M00

(*** ASIGN CORRECT MCODE FOR PALLET FACE ***)

M00

M54 (or 55 etc)

 

If the datums on each station are fixed and known, the XYZB can be in the M code prog to save on setting time? 

[absolute technologies]

 

 

How do other shops handle this type of situation?

We read the work offsets in with at the beginning of the CNC program using G10. Every job has G54.1 P1 for B0, P2= B90, P3= B180 & P4= B270 then P5 etc for odd angles, it's always the same . for every job and less confusion because every job has the same work offset/B-axis table position scheme, furthermore pretty much fail safe reading the work offsets in with each job. In this case where they're doing tombstones work on different faces, the operators would only need to edit the G53 B work offset at the beginning of the program because one time the fixture may be B90 then next time its' at B270 or whatever

 

Cheers!

Len

[Matthew Hajicek - Singularity]

The problem I see with that approach is that the same programs are used on different machines, which will have different work offset positions for each station.  Also, many of the programs are 2nd ops and require the part to have been probed in.  They run a probing cycle before running the main.

[Newbeeee™]

The problem I see with that approach is that the same programs are used on different machines, which will have different work offset positions for each station.  Also, many of the programs are 2nd ops and require the part to have been probed in.  They run a probing cycle before running the main.

By assigning a M code prog with that prog in each machine, it's machine specific (different) datums can be within each separate prog.

We did this with a customer of ours when we setup their machine shop - 3x vmc's with manual pallet changers. The pallet change position for each machine is called via M100.

Each M100 program within each machine, has slightly different co-ordinates to match the pallets.

Doing this allowed for the same prog in each machine with everything (prog wise) identical between all.