some tool setting questions

[awjareme]

In our training (RH33 centurian 7) we were shown to put the machine in HDW mode and z-down to our tool setter then press Ztool and hit enter then enter the dia. and repeat for all tools (then never worry about it again unless a tool is changed). Looking in the manual there is a TLSET on the main screen, which does a similar thing but also asks for the tool setter height. Which way is the proper way to set tools. What does the machine do differently when it knows the setter height?

Also when setting G-54x,y,z in HDW mode (we are using a remote HDW) i use the edge finder and setting G-54x and y is straight forward and easy, when it comes to setting the Z can i use the edge finder or is it better to use a tool in the program? also when i am at my z height we were told to go to Main-param-coord-G54 edit then hit M-Z? Is there a simpler way to do this? Why is there no G54-Z button in HDW mode? Why is there only a ZTOOL option? Also because of confidence levels (we are beginners)we change the Z- height of our tools using H-OFF by a positive# to dry run the program first for verification. Is there a simpler way to dry run a safe distance above the part. I'm worried about crashes if someone forgets to set the H-OFF back. We haven't run too many multi tool programs yet, but i have tried a couple drill/taps and the tap ended up inches off in the Z. So i have been running seperate programs and setting each tool as above before running that program, which brings up my last question. I can drill in rows/columns, but where the heck is the tapping option for rows/columns? i can only find bolt circles and single holes. makes for a lot of pages when doing lots of holes.
Thanks for any help, wish this manual was a bit better

[chipsinpan]

I am suprised nobody responded to this basic query . I am fluent on Cent 5 only , but the basics still apply .
do not use the edge finder to set Z .
while X & Y g54 ( g55,g56,g57,g58,g59 ) are work coordinates for table movements , Z is a variable location depending which tool the control assumes is in the spindle . So the safe way to set Z or Ztool is to do an MDI tool change ( M6T1 ) and then the control knows you are setting for tool #1 ,
then use HDW to physically move the tool tip down to the Z location you want , and enter Ztool 1 , dia / z zero ( you really only need to enter the diameter if it is a cutter that will use cutter comp ).
When I first learned to run my old Partner , I also ran the first time with no tool in the spindle . But you can also run VERIFY , which will just run the tool path on the screen , but not the actual table movement .
Then you can RUN / HDW /START, which will allow you to progress through the program as you turn the handwheel . This allows you to simply stop turning the HDW to stop the program when you sense a crash is coming .
It will NOT allow you to crank the HDW back to get out of the program .
You need to press HALT / ESC / then JOG to get out .
I didn't answer all your questions , maybe someone else will fill in the blanks .

[ZZZZ]

The "correct" way to set Tool Length Offsets is the one that works for you.

You can use the Z-TOOL button in HDW, or you can use the RUN - TLSET technique.
The HDW way usually requires you to go to MDI to change tools before you can use the HDW Z-TOOL button while TLSET does it for you. TLSET also accomodates the height of your setting device: shim stock, piece of paper, gage block, 1-2-3 block, dowel pin, electronic or dial gage.

I recommend new users use the TLSET technique, it eliminates some of the mistakes you can make.

Do not confuse setting Work Coordinate Offsets with setting Tool Length Offsets. There are 99 TL offsets and they will work in all 60 WC offsets. I caution all users to be very careful when putting values in the Z registers of the WC offset table.

All offsets are additive, so if you have both TL offsets AND WC offsets for Z, you stand a better chance of crashing into t he top of your part.

As you become familiar with the machine/control, you may want to investigate the tool setting options listed in the MISC setup parameters.

Good luck and be careful, I have seen some scary crashes caused by incorrect tool setting.

[awjareme]

When you say you have a better chance of crashing if you have tool length offsets, and work coordinate offsets. Do you mean its better to set every tool you use for a particular part to that part?

I was doing a drill/tap and broke a tap. Originally i touched the drill and tap to the tool setter, then set the drill to the work surface. When i ran the program the tap (which is a lot shorter) followed to the correct offset. After i broke the tap, i only had a different brand on hand so i called up the tool and re-touched it to the tool setter (thinking it will take into account the new tap length). When i re-ran the program the drill came to the correct offset, but the tap tried to go down to the tool setter height which was 4" lower than the part. ( i was watching distance to go and caught it). Does this mean everytime i need to change a tool, i need to reset everytool in the program?

Also say i chip an insert in the middle of a program, is there a way to handwheel away so i can take the tool out and change an insert, then resume in the program? I can only figure out how to advance through the program with the handwheel. If i end up at the jog screen location the entire program needs to be re-started.

Sorry for the basic questions, but the manual is a bit tough to use for trouble-shooting.

[ZZZZ]

When you say "Originally i touched the drill and tap to the tool setter" do you mean a Renishaw contact or laser tool setter or do you mean a manual tool setting device such as the battery powered gizmo with the red lights?

This explanation only works with manual tool setting, automatic tool setting uses a different technique.

The Tool Length Offset value stored in the Tool Table is the distance from Z axis at home position down to the Z-Zero surface on your workpiece. You want to set all the tools for a set-up from the same Z surface so the tools are all relative to each other. When you change set-ups, use theTLSET macro to re-set the tools you need for the new set-up.

The X and Y Work Coordinates do not affect the TL offsets but a value in the Z axis WC offset DOES shift the whole tool table up or down.

If you want to stop a program in the middle, you can press the HALT button. You can then stop the spindle, jog or handwheel the head up and move the table around. As long as you don't do anything to change a machine parameter (change the length of a tool, move the part, etc) you can RESUME the program. The machine will rapid to the X-Y position first, then rapid to the R-Plane above the halted position. Just changing inserts wouldn't change the tool's length so you would be able to resume the program. People use this feature to brush chips away, move clamps, etc.

[awjareme]

I was using one of those battery, red light contact gizmos. So i set every tool in the changer to that height(2.0") using TLSET. After doing all this i touched the drill to the work surface (approx 6.0")using the M-Z in PARAM-COORD-G54-EDIT. The hole drilled, then the tap came down to the proper height as it should as the machine knew all the offsets. The issue was when i changed taps i used the tool setter on the table using TLSET, agian thinking it has a different length, so the machine needs to know this. I then re-ran the program and the drill stayed with the workpiece (6.0"), but the tap tried to run at the tool setter height(2.0")????.
Kind of like all the H-OFFs changed for every tool when i touched the part with the drill, but the tap got its HOFF from the TLSET, and its value never changed by the 4.0" when i re-ran the part. Almost like when i change a tool, i have to re-do the entire carousal. Normally this wouldnt happen with inserts, but when i use collets its a pain.

Also i cannot move the table after hitting HALT. If i hit HDW it only cycles through the program. I have to his ESC, the JOG, then the whole program is lost. I noticed in my PARAM-SETUP-POWER 2nd and 3rd Handwheel encoder Axis are set to 0 and 0. I have the remote handwheel and by the manual looks like these values should be at 4,5. Could this be the problem? I was kind of nervous messing around in there.

[ZZZZ]

Generally, there is no need to do the PARAM-COORD-G54 thing, doing so just adds another offset to the mix. When you went to set the second tap, you had a G54 Z offset active that was not active for setting the other tools. Effectively, all the Tool Length Offsets DID change when you add the G54 Z offset.

Please, set the Work Coordinate Z offsets to zero and try it again. Only use the Z offset if you have a two vise set-up or something similar.

After you HALT the program, ESC all the way back to the Main Menu before going to Jog or HDW. The HDW next to the HALT button is the Handwheel Run feature.

Does the remote handwheel work normally when you are in Main - HDW? If so, don't mess with the parameters

[awjareme]

O.K. got the handwheel thing figured out, thanks alot. Pretty basic, but if you've never been showed it before, its not the first way that comes to mind.

As for the tool setting. Are you saying that instead of using the tool setter. Set up the tools used in each program to the work? I basically had in mind that using the tool setter set all the offsets to an even plane, then when setting the WC all the offsets moved to that work height. Then from then on any tool set to any WC, all others will follow? And whenever i used the TLSET it would automatically enter that tool to the current WC. But doing it this way is not correct and more likely to cause a crash? I'm sorry for the basic questions, but it is a little tricky trying to figure this out on my own. Especially now that i'm producing parts using what are probably bad habits, and trying to go back and get the basics straight. Hopefully i can look back in a month and think what a stupid question i asked. Thanks for your time.

[ZZZZ]

It sounds like the guy that trained you to operate the machine didn't do a very good job.
These things (and lots of others) should have been covered at start-up.

This is from the SET-UP parameters MISC section of the manual:

G5#-Z in Handwheel Yes will allow the G5#-Z key in handwheel.

Tool Setting If set to any tool the jog and handwheel tool setting routines will prompt the operator for the tool # being set. If it is set to current tool the control will assume the active tool # is the one that is being set.

Tool Setting Use Work Offsets If set to No, the position given by the operator is relative to home. If set to Yes, the position given is relative to the work offset (this is useful for tool setting off the table and using a Z work offset to the top of the part).

[sportybob]

ZZZZ is correct.
just a note about using a "tool setter" "red light blinky thing" mostly used by our friends north of the border. but is "can be" a good work practice.
when setting the Z the "tool setter" that is mounted to the table and usually located below the part "zero" "on the tabel below the vise".
When using this meathod you would enter the difference between the top of the part and the top of the "tool setter" is is a - number.
Doing so adds the value of, if you do not enter a -z depth, it goes + and drills / mills up instead of down. hence less tool chashes.

You do need to figure in the top of the "tool setter to the top of the part. Annoyning at first, but once you get used to it. far less crashes will occure.

sportybob