G10 AND G52'S ON HAAS

[motor-vater]

Back Story: No need to read unless Bored....

Some of you know I took on the position of programming for a 40 year old Job shop that has employees that have been here for 30+ years, change has been hard to implement but I have been told on numerous occasions thats what I was hired for and they will have to keep up with it or get out.. lol They have beat me down as far as Compensation at the control, because wear just proved to hard to implement and considering there catalog of 1000's of programs are all at control, I gave in. Not the problem. Problem is all of their old programs while functional are hack jobs and require way to much messing with on a change over so I have been assigned a new task. Every time a old program is called to the floor it is now my job to go through it and try to eliminate the guess work. Some examples are things like instead of calling a chamfer mill a chamfer mill, its in there as a .125 endmill.  ( A machinist told me just look at the the Z depth and you will know its a chamfer mill... lol). Best part is the machinist also has to double the depth in the diameter offset column for it to work right, if its Z-0.030, the diameter offset needs to be set at 0.060.. But the one that kills me the most is there work offsets. All machines are haas with renshaws. But the part zero maybe anywhere. Could be Z-.150 from top of stock, could be X 1 inch from the left side of stock, etc... Much time is wasted trying to figure this out every time they pull a job out of the archives, and dont get me started on the tool list issue, so much has been programmed at the control that you have to read through the whole program to find out what tools are required... So, I have been manually editing a bunch of Gcode which I really actually enjoy, being a 12 year veteran of MCam and having the right posts has really enabled me to not really have to know G-code as well as I should. I now add a tool list to the top of each existing program, change the tool descriptions to match the required tools, and even add in some comments to help quickly set the work offsets for next time. I started plugging in G10's to set tool offsets for things like the chamfer mills and the boss thinks I'm a rockstar.. Lol

 

The Question:

So in order to utilize the renshaw system I would love to just quickly probe parts and use a G52 to modify the work offset to catch up with what ever part zeros they used in the program. I dont think this is a problem. What I am concerned about is I think I need to use another G52 to move back to probed zero at the end of a program, or it will just continue to move the offset every time the machine is reloaded, Correct? So how does that affect the programs ability to reset. Example Running program and a tool breaks, or they use op stop it and decide to offset the tool more to maintain a clearance and re run from there. When they restart in the middle of a program whats gonna happen? Common practice here is to stop the program, change the offset, hit reset, then scroll to what ever tool it was and press cycle start (recut same hole). Should I use G52's at the beginning and end of every tool, or does the concept of G52's not make sence for my current situation? As always thank you for you help..

[Guest]

Some near 20 years ago, I stepped into a position not thoroughly unlike yours...change needed to happen....

For the 1st few months, I kept everything as it had been running and I built myself some time to get ahead...

At that point, I started to reprogram EVERYTHING, I removed old paperwork, old programs. I eventually rolled out the 8 file cabinets that all of the old setup sheets resided within.....there was some push back from the floor, they were essentially told you can work with us or leave, the choice is yours...I think only 1 person left....IIRC

Implemented probing, modular fixtures, and new programs....it took the better part of a year.....after 2 years, the numbers the shop was doing spoke for themselves...1st pc acceptance way up, setup hrs down, # of jobs through shop way up, even though I basically stopped using 2 old Fadals, we implemented a tool crib position which in turn paid for itself in saved setup time alone......

Make a plan......implement plan......modify plan(as needed)....refine plan but mostly, plan to do what you need to do to help the shop succeed but most of all modernize

Edited June 8, 2018 by Guest

[huskermcdoogle]

Why use G52 at all?

Just probe and shift the work offsets needed.  No bs or trickery required.

Though to answer your question.  In theory G52 should cancel any time you command a work offset, upon pressing reset, or after an M30.  For safety sake, you could command a G52 X0,Y0,Z0 in your program header, and that would cancel it as well.  I rarely use G52, and if I do it is pretty only to get a part within tolerance when working multiple faces on a 5 axis that has calibration issues, and I don't have time to figure out where the error is, or how to correct it (usually a mechanical issue).  

On the subject of fixing everything to improve the situation.

I have never been in a situation like yours where I was tasked with fixing everything, but I have been in a few shops where the general state of the union was the same.  It's super frustrating, even sometimes beyond frustrating, when all you have is a program to work from.  Thankfully in those days, everything was hand written, the programs had a consistent format, and generally speaking there were enough comments in the program to figure it out without a lot of pain.  The challenge was, there were no tool sheets, or any premonition of what the program was supposed to do, or any confidence that the job was "proven", as you had no idea if you had the right tool, or projection.  Inevitably it would take a few days to get a job up and running.  Lots of dry run time, single blocking, clearance checking.  Just plain painful.  Great learning experience as I was a greenhorn at the time, but painful, very painful.

I, right now as we speak am shoring up documentation for all of the possibly recurring work I have done in the last four years.  I have taken the time to customize our active report tool sheet output to fit our needs, and am creating detailed drawings of the setups.  Time consuming, and I should have likely done them before now, but I would work on them, and then be pressured to drop it before I finished and move onto the next project, as a machine as sitting waiting for the next job.  I was doing 99% of the setups, and it wasn't a big deal, before I would go do a setup to just glance at the mastercam file, print a tool sheet, and then go set it up.  Easy peasy, but my time has become to valuable, so now I have to get the information out of my head, and on paper.  Easier said than done.  It's the things you take for granted from your training that are hardest to convey in a setup sheet.

[mkd]

been using haas for 20 years. never once used g52

maybe my loss.

or not

[huskermcdoogle]

5 minutes ago, mkd said:

maybe my loss.

or not

like more on the "or not" side of things....

[Matthew Hajicek - Singularity]

I found myself in a very similar situation almost a decade ago.  The solution was to THROW AWAY all the old programs and documentation and reprogram everything from scratch.  Cycle times were cut at least in half, and sometimes by 75%.  Tool life improved, part acceptance increased, programs became reliable enough to run unattended overnight.  If you have to go over each program with a fine tooth comb and fix it anyway you might as well.

[huskermcdoogle]

1 hour ago, Matthew Hajicek™ - Conventus said:

The solution was to THROW AWAY all the old programs and documentation and reprogram everything from scratch.

Unless it is a dead simple part, this is likely the best scenario regardless if it has good documentation and whatnot.  I wonder what a good time frame is for this.  I would bet that almost anything 10 years old at this point is a good candidate, at least for a look at the process approach and roughing strategies.  But 10 years from now the only obvious potential I can see for repogram would be for new machines or new spindle tooling.  We likely aren't going to see an order or magnitude faster roughing strategy come through CAM improvement in the next decade such as we did with dynamic paths, in special cases, maybe.

[JoshC]

23 minutes ago, huskermcdoogle said:

Unless it is a dead simple part, this is likely the best scenario regardless if it has good documentation and whatnot.  I wonder what a good time frame is for this.  I would bet that almost anything 10 years old at this point is a good candidate, at least for a look at the process approach and roughing strategies.  But 10 years from now the only obvious potential I can see for repogram would be for new machines or new spindle tooling.  We likely aren't going to see an order or magnitude faster roughing strategy come through CAM improvement in the next decade such as we did with dynamic paths, in special cases, maybe.

I respectfully disagree with this opinion, A lot has changed in the last 10 yrs in manufacturing, and i expect the next 10 yrs  to come with have just as many changes and technological improvements as the last 10 yrs has.

Everyone and their brother is working on the Latest and greatest of everything, we are always trying to improve everything and even though we do not know what types of crazy new tooling, machines, Software, etc. is coming in the future my opinion is the world is not slowing down and the drastic changes that had happened over the last 10 yrs will be just as drastic over the next 10. 

On a side note i recently seen a video the Tool Vendor Emuge provided on their new threading technology called Punch Tapping which makes me wonder if the way we have been tapping holes for the past decade will remain the same method for threading holes in the future.

[Newbeeee™]

14 hours ago, JoshC said:

On a side note i recently seen a video the Tool Vendor Emuge provided on their new threading technology called Punch Tapping which makes me wonder if the way we have been tapping holes for the past decade will remain the same method for threading holes in the future.

Josh - you're 2 years behind the curve LOL

I wholeheartedly believe there will be improvements as time ticks along, but I can't see anything as revolutionary as the trocoidal paths. This strategy has truly been revolutionary - probably as revolutionary from HSS to Carbide.

[jlw™]

I have never used G52 in my entire life.

[Clarence L Cook]

I use G52 all the time.  I have four Haas verticals and a Makino horizontal that I use G52.

Most of my work is vise work on the verticals and I make fixture plates for the horizontal.

I have the G52 set to a common Z location, typically the bottom of the parallels.  Then I add the parallels and the material height, if any, to the specific work offset.  This allows me to program G10 Z values in Mastercam which gets set the first time the program is run and not again.  This allows me to move the part to any of the verticals that can accept it, because each of the G52s are specific to the machine.

Check setting 33 on the Haas.  If it is set to Fanuc, then using G52 makes no sense as it gets reset to zero on a reset, M30, etc.  Setting 33 would have to be set to Haas, but the Renishaw macros don't like it and alarm out.  I had to modify my Renishaw macros to bypass the alarm message.  I know it is a danger, but I haven't come across an instance where it has been an issue.  I also don't use the Haas quick codes, I only use the macros imbedded in the programs, using manual entries.

Good luck with updating your programs.  I am currently doing the same thing to incorporate all of the process changes I have implemented, ie probing, mid cycle starts, etc.

[Newbeeee™]

Similar but different, is a way 3 vms were programmed at an old customer of mine. They were all fanucs with twin pallets and rather than set all machines identical as we did (grid shift etc) they called a M100 datum program.

This was effectively a 9000 protected prog named via m code (look at the parameters and they're assignable like prog 9001 is usually M6 for toolchange).

So the one base prog was grammed and could go on any machine as within the M100 prog was the G54 xyz with their related values.

It worked okay, and when a machine had the thrust bearings replaced, it just meant that the table was reclocked and the value in the M100 prog amended.

[LucasGC]

On 6/9/2018 at 5:42 AM, Newbeeee™ said:

Josh - you're 2 years behind the curve LOL

I wholeheartedly believe there will be improvements as time ticks along, but I can't see anything as revolutionary as the trocoidal paths. This strategy has truly been revolutionary - probably as revolutionary from HSS to Carbide.

4 years -