"h" tool length offsets

[zappafanx]

Komo vmc 50/160 with GE fanuc series 18i-M controls. I'm an operator and was wondering if there is a parameter setting to avoid losing tool length(H) offsets at reset? thanks

[crazy^millman]

No. That is a function of the machine. I have questioned it myself over the years, but they are dumb machines and you must teach them the basics every time. It is also a safety feature of the machine.

[GoetzInd]

 

 

avoid losing tool length(H) offsets at reset? thanks

[specv]

Im not familiar with the machines but can you have a sub program for the tool offsets and just read the program again after reset? That is how we get our gage lengths into our machines.

[Allan]

There is a parameter setting on Fanuc that controls if the tool length is cleared when reset is pressed.

 

Allan

[Grievous]

Check in parameter manual:

- #5003 LVC, LVK, CCN

- #5001 EVO

- #3402 CLR

- #3409 CFH, Cxx

Save actual values and give it a try

[mkd]

Just be thankful it's not a 6M that adds the value to the old value if the machine reads the H a second time, without hitting reset (not once but twice).

[Matthew Hajicek - Singularity]

Ouch.

[zappafanx]

Thanks guys, I appreciate the replies all. If the programmers had put the necessary redundant  information in at each "machining area" I wouldn't have had to ask this question. The format of our programs is not very operator friendly.   As it is now, we have to go back to the very beginning of the program and satisfy all the g, m, s, h, a, etc.  codes(and some are scattered in other ares of program) to rerun a particular "machining area". And of course if you happen to forget or miss just one of them, whammo! and that's what happened to me last week. We have thousands of programs formatted the same so they're not going to go back and fix them. Struggle on.......

 Happy New Year!

[zappafanx]

Grievous74

looks promising. I'll relay info to our programmers and engineers. Thanks again!

[jlw™]

I force tool change on almost every op just to make it easy to restart. I only have G53G90Z0. as my safety moves. All of my machines have safety moves for TC in the TC macro. So it only costs me a Z home move. If they want it to keep running just turn off op stop. I also comment the scheiße out of paths as well. No such thing as too much info.

[Guest]

Zappa, a little time spent on tuning post processors is worth it's weight in gold.

[RaiderX]

program restart can be your friend but better know the ins and outs of it. I used to hard code by hand g43 h and d in area's that needed multi re run proofing etc.

 

just a band aid not a fix.

[Newbeeee™]

Zappa, a little time spent on tuning post processors is worth it's weight in gold.

A lot of time spent tuning a post is worth even more!

[Sticky]

Just be thankful it's not a 6M that adds the value to the old value if the machine reads the H a second time, without hitting reset (not once but twice).

 

Sounds like you weren't canceling the length offset (G49).

 

I don't have a problem with reset erasing G43, but if you are going to keep G43 at reset then I would highly recommend using G49 at the end of a tool. Which is good practice anyways.

[Guest]

I ALWAYS use G49 at plane changes and the end od the tool and I also use G53 instead of G28.

 

JM2CFWIW YMMV

[jlw™]

Same here.

[Sticky]

I ALWAYS use G49 at plane changes and the end od the tool and I also use G53 instead of G28.

 

JM2CFWIW YMMV

 

Why do you cancel at a plane change if you are using the same tool? I've always kept G43 active until a tool change.

 

I used G53 when I first started programming (which was mostly by hand), but for some reason when I switched to Horizontals I switched to G91 G28, emphasis on the G91 part. But now I can't remember why?

[civiceg]

Some controls cancel tool length or work offset when calling up a G28. 

[jlw™]

You can't activate/cancel G68 or G68.2 with G43 active and need the cancel at plane change.

[Newbeeee™]

Why do you cancel at a plane change if you are using the same tool? I've always kept G43 active until a tool change.

 

I used G53 when I first started programming (which was mostly by hand), but for some reason when I switched to Horizontals I switched to G91 G28, emphasis on the G91 part. But now I can't remember why?

Old hori/control?

Only newer series can handle G53

EDIT - when I say newer controls, all things are relative...

[Grievous]

You can't activate/cancel G68 or G68.2 with G43 active and need the cancel at plane change.

Well...sometimes you can.

..this a proven program from last week. Sometimes is just about settings on controller

N50T50(2" HF INS EM)M06(MAX=Z29.6005 | MIN=Z-.4)M01(CORNER 1 CUT EXTRA-WEAR COMP/DIA2.)(EXTRA ON XY=0. / EXTRA ON Z=0.)G54G90G00G43.4H50D50Z8.X-24.Y23.A0B0C0S900F60.M03Z8.M07A-.897B7.287G43.1G68X0.Y0.Z0.I0.J0.K1.R97.034G68X0Y0Z0I1.J0.K0.R7.342G90G00X25.766Y21.8528Z5.2506X17.3648Y19.944Z5.Z4.32G01Z4.2601G41X17.3437Y19.8462..G01G40X24.5165Y17.7708G00Z5.X25.766Y21.8528Z5.2506 (CUT CORNER-1 F1-COMPUTER COMP/DIA2.)(EXTRA ON SURF=0./EXTRA ON CHECK SURF=.01)G69G43.4X-24.Y23.Z8.A0B0A-19.388B-48.557G43.1G68X0.Y0.Z0.I0.J0.K1.R244.851G68X0Y0Z0I1.J0.K0.R51.366G90G00X-10.6205Y-13.417Z29.6005X-4.3355Y-10.4343Z24.Z23.2374..G00Z24.X-10.6205Y-13.417Z29.6005M09G69G91G49G53Z0M05G91G0G28Y0A0B0C0M01..

[Sticky]

Some controls cancel tool length or work offset when calling up a G28. 

 

I can't say I've ever seen that. By 'cancel" do you mean calling G49 and switching to G91? I can't see how you would actually clear the work offset register without making a macro to do it, which would be insane.

 

You can't activate/cancel G68 or G68.2 with G43 active and need the cancel at plane change.

 

I just double checked some of my programs and I am definitely calling G68 while G43 is active. Sounds like it's something you should be able to change with a parameter.

 

Old hori/control?

Only newer series can handle G53

EDIT - when I say newer controls, all things are relative...

 

Well the first machines I was using G53 on were early 80's. The machines I run now are much newer and certainly capable of using G53, I think I have G53 in the pallet and tool change macros. I might not have had a good reason for switching, I'm not sure if I will be able to remember or not.

[Newbeeee™]

The funny thing is we modded our post to call G28 (no G91) as the post just repeats the Z value for the last retract.

So the path retracts and goes home eg

G0 Z25. M09

G28 Z25. M19

 

I didn't want our machines to use G91 because I hate going into incremental.

But we didn't use G53 for some reason...

 

HAHAHA - just quickly tried it on a machine - the reason why we didn't do it was because the green 'home' light would not illuminate using G53.

The machines function okay but I guess there's a ladder issue.

[Guest]

You can't activate/cancel G68 or G68.2 with G43 active and need the cancel at plane change.

:

 

And since 90% of the machines I deal with have this function, that's what I do.