Results 1 to 21 of 21

Thread: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

  1. #1
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Hi,

    I have a feeling that I'm going to have to start out every post with a "I"m a Lean guy and not a CNC guy" so hopefully people can give me answers that I understand. I definitely appreciate the wealth of knowledge a forum like this has to offer.

    So, I'm doing a set-up reduction at a client (an OEM) on an old Dahlih MCV-760 (40 taper 3-axis vertical) with a Fanuc control (not sure which model, but I'm sure we're talking 80's tech). Safe to say there is a knowledge gap, I know a bit about CNC progamming and operations and they are definitely not as skillful as they should be.

    The machine is running a family of parts that each have their own dedicated fixture that doesn't come out except for maintenance (4 fixtures total, 4 parts total). In that regard, the set-up is short, you don't have to change out fixtures. Some of the tooling is common. What confuses me is they are doing a lot of tool offsets measured in the machine and it also appears they have to do this every time a tool is used on a different fixture. This turns an otherwise 1-2 minute changeover into 5-7 minutes. So, my questions are:

    1. Is there a cheap way to measure tool offsets so you can load this into the machine? Some of my "more up to date" clients has pre-setters that print out all the info and you can load it up while the machine is running parts. They have a limited budget.

    2. Let's say you had to stick with doing this manually (measure int he machine), shouldn't you be able to, once the offset is measured on one part (for a given tool), use the same offset for the other parts on other fixtures using the same tool? They use some sort of fixture offset (G92?), could this compensate for z-axis differences so the same offsets could be used?

    Hopefully I'm asking this question properly. Just to sum up, I'm trying to find them the best way to measure the offsets, ideally "off the machine" so they can be loaded once and used on any program within the machine so they don't have to be adjusted again until the tool is changed out or sharpened.

    Thanks!
    Biederboat

  2. #2
    Join Date
    Apr 2009
    Location
    Kansas
    Posts
    90
    Thanks
    0
    Thanked 8 Times in 8 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    You could measure the tools with a height gage out of the machine load the the lenght into your offsets page. Then just touch one tool off the Z0 point on your part or fixture and then put that number in a G54 through G59 work offset if this machine has them. or you could measure them in the machine and do the same thing then when you can use the same tool lenght for all the fixtures and just use a different work offset. the next option I can think of is to measure your tools off each fixture and record them and take those numbers and put them in the program along with a G10 command and it will load the right offsets from the program each time it is ran and last if you under stand how to use marco programming you could put these offsets into vairibles and call the up from the program all of these Ideas have there good and bad points the work offsets is your best bet I think then the G10 if you have not used marco programming then that will take a lot of learning

  3. #3
    Join Date
    Mar 2010
    Posts
    171
    Thanks
    0
    Thanked 18 Times in 17 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Your machine may not have macro-programming feature if it is an old model. G10, which is again an optional feature, might be available (if it is not available, you will have difficulty in simplifying your task). Macro-programming offers more flexibility, but G10 also can be used for your purpose. I am assuming that G10 is available.

    There could be several ways. I would explain one method which is very simple (though not the best method):
    Define one tool as a "standard" tool, and complete the work-offset procedure with this tool, in, say, G54. As long as you need to use this tool, no length compensation (G43/G44) would be required, if you are in G54. Now you need to know the difference in length between this tool and the next tool you are going to use. If the next tool is smaller by, say 5 mm, enter the following in the beginning of the program
    G91 G10 L2 P1 Z-5.0;
    G54;
    (no need to use G43/G44 now, for this tool)

    At the end, insert (for reverting back to the original setting)
    G91 G10 L2 P1 Z5.0;
    M30;

    If you do not want to edit your programs, you can also execute G91 G10 L2 P1 Z-5.0 in MDI mode, before executing the program, and G91 G10 L2 P1 Z5.0, after the program execution is over.

    Of course, I have not talked about wear compensation.

    G92 is not a good method, because its effect remains valid in the current machining session only. In a subsequent session, you would again need to bring the tool to the desired Z0 position and command G90 G92 Z0.

    Sinha

    Edit:
    For four fixtures, use G54, G55, G56, and G57 respectively.
    Last edited by sinha_nsit; 09-25-10 at 04:14 AM.

  4. #4
    Join Date
    Oct 2008
    Posts
    650
    Thanks
    3
    Thanked 97 Times in 78 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Interesting post you guys have over here...there is a phrase in Biederboat's comments that strongly called my attention: "They use some sort of fixture offset (G92?)".

    Some time ago I was going crazy trying to find out where the G54 ~ G59 pages were on an 80's Fanuc controller, I never found them.

    What I actually found, after doing a lot of research, is that the controller I was fighting with, was a Fanuc 6M-A, wich never had the G54 ~ G59 "option" (You gotta think early 80's) G54 ~ G59 were able at the 6M-B and later controllers.

    Once I learned that, I used and recommended (for this machine) what actually called my attention today...guess what? <<<G92>>>.

    But of course, it's just an idea of the issue you might be facing...think early 80's...

  5. #5
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    There are many ways to do this and more info on how your machine is setup and the features it has will need to be known.

    80’s it is probably a Oseries control. The older Ot series did not all have the G54-G59 work offsets. The Om series did. It was an option however.

    Ok so I ass u me that since you are doing offsets all the time that you do have a tool offset page. How are you controlling the height or location of the 4 fixtures that you have on the machine? G54-G59??

    Tool offsets are simple and you should never have to keep touching off your tools unless they break or you change them. If your tools can reach the table face then you should touch all of them off of that surface. Use the measure function (if your control is equipped with it) or manually calculate the offset.

    Simple breakdown would be that you have a distance from spindle face to the table. If you were to program G0Z0the spindle face would move to the table face (not all machines are setup this way but this is an easy example). Now if you were to do a tool offset to the table face and activate your tool offset with G43H()Z() and program G0Z0 then the tool tip would go to the table face. Now you need to compensate for your fixture height. This can be put in the G54-G59 if you have them or they just may be hard numbers in the program. So lets say you had the height of each fixture in G54-G59 and you touched T1 and T2 off the table face.

    G43H1Z3.
    G0G54Z1.
    This sends T1 1.” Above the fixture in G54. If you replaced the G54 with any of G55-G59 it would send T1 1.” Above each of those fixtures. If you replaced T1 with T2 it would do the exact same thing except with T2.

    Here is another thread that may help where this was discussed as well.
    http://cnc-professional-forum.com/pr...ro-toyoda.html

    Hope this helps. Give us some more info on fixture height and if you have G54-G59 and I can tell you exactly how to set up the machine.

    Stevo
    (The opinions in this post are my own and not those of machinetoolhelp.com and its management)

  6. #6
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Thanks Guys, I'm trying to get the model of Fanuc control. I have a pic but it won't let me post (I'm too new!). If I get it soon, I'll post the model.

    Thanks,
    Biederboat

  7. #7
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    It should say right on the control most likely by the CRT. If not you can locate it in the power cabinet. There should be a sticker with the model and serial number or the control.

    Make sure that you get us the rest of the info that is more important than the control model.
    Do you have tool offset registry?
    Do you have G54-G59?
    How are you reading the height of all 4 fixtures when programming?
    When you program G0G90Z0 does the spindle go + the table or – to table face?

    Stevo
    (The opinions in this post are my own and not those of machinetoolhelp.com and its management)

  8. #8
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Thanks, it says I need 6 posts, this should be #5 so I'll do a short one again and then maybe I can post!

    BB

  9. #9
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Here's post #6!!! Crossing my fingers!

    BB

  10. #10
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Here's a photo of the control. I'll work on trying to get the other answers to Steveo's questions but maybe this will help in the mean time.

    BB


  11. #11
    Join Date
    Oct 2008
    Posts
    650
    Thanks
    3
    Thanked 97 Times in 78 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Looks like a 10M to me...

  12. #12
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Quote Originally Posted by Sinumeriko View Post
    Looks like a 10M to me...
    I agree.

    BB,
    Do you have the answers to the other questions I asked above?

    Stevo
    (The opinions in this post are my own and not those of machinetoolhelp.com and its management)

  13. #13
    Join Date
    Oct 2008
    Posts
    650
    Thanks
    3
    Thanked 97 Times in 78 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Stevo,

    BTW, thanks for the answer to that PM from the other day.

  14. #14
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Hi guys, back again.

    Interesting guess on the controller. There are two machines that are very similar. One has a 10M (the one in question), the other an 11M. As I recall (and backed up by my client), they say the photo is of the newer machine and thus an 11M. In any case, the machine in question is a 10M. Now for the other questions (just a quick not that someone there is helping me get the info, I don't have easy direct access to the shop):

    Do you have tool offset registry? Yes, assuming this is the H1, H2, etc.

    Do you have G54-G59? I am told only G54.

    How are you reading the height of all 4 fixtures when programming? Their answer: Fixture height is read by taking the difference between the reference tool post and the fixture. My addition: I didn't think they had a "reference tool post" on these fixtures. They do have a " reference post" on the other machine (the one with the 11M that runs entirely different parts but these parts may migrate over there in the near future) so there may be some confusion here.

    When you program G0G90Z0 does the spindle go + the table or – to table face? Motion depends on program and established zero (as I'm told).

    I really appreciate this help. Just so everyone knows (I think this is important), I'm not really charging them for this information. I don't want someone to think I'm getting free info and charging my client for it.

    Biederboat
    Last edited by Biederboat; 09-27-10 at 11:14 PM.

  15. #15
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Ok where to begin.

    If you have G54 you have G55-G59. I have never heard of a machine that has only G54. G54-G59 is an option and to the best of my knowledge you activate all or none.

    I like to set up my tools to use gauge line offsets. IOW it is the actual length of the tool that goes in the offset registry. This helps standardize the process. This will help visualize the tool so when you do a tool offset you don’t have some crazy -24.1025 to input in the registry when the actual length of the tool is 6.512”. This is just a preference and not a rule so I am not going to go into much detail on how to set that up right now.

    First thing you need to do is offset the tools off the table. If you have the “measure” function on the control you will not have to calculate out the tool offset. The tool offset manual calculation will vary depending on where you have your “home” position of the machine set up to.

    Now that all of your tools are set to the table you can program anyone of them to go to the table top by activating the tool offset and then programming them to go there. Don’t get tripped up by having a value on the G54 Z. G54 is the default on the Fanuc controls so even if you don’t program a G54 it will still take in account the value in G54 when you go to move the machine. I typically never use G54 for this reason so I leave it at 0,0,0.

    I drew up a quick sketch of a tool, spindle, table, and fixture to give you a visual. This is taking G54 to all zeros. Now you touch off T1 on the table face and set it in the offset registry. If you activate the tool offset with G43H1Z() and program G0Z0 the tool tip will go to the table face. Now if you program G0G55Z0 the tool tip will go to the top of fixture #1. If you program G0G56Z0 the tool tip will go to the top of fixture #2 etc. The offset for T1 never changes. If you were to offset T2 to the table and program G55Z0 T2 will go to the top of fixture #1 the same as T1 did.

    I hope this helps.

    Stevo
    Attached Thumbnails Attached Thumbnails offset sketch.pdf  
    (The opinions in this post are my own and not those of machinetoolhelp.com and its management)

  16. #16
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Quote Originally Posted by Sinumeriko View Post
    Stevo,
    BTW, thanks for the answer to that PM from the other day.
    My apologize I don't remember what I helped you with but as long as it helped

    Stevo
    (The opinions in this post are my own and not those of machinetoolhelp.com and its management)

  17. #17
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Hi Stevo and all,

    Hey thanks for sticking with me. In my limited experience, everything you said makes sense and I was wondering about the G54-59 myself. I've got to digest it a bit more to make sure I fully understand and can explain but this has been a really great forum and everyone's input greatly appreciated.

    Biederboat

  18. #18
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    You’re welcome.

    Ask as many questions as you need to. We will answer the best we can.

    Stevo
    (The opinions in this post are my own and not those of machinetoolhelp.com and its management)

  19. #19
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    In my limited ability to explain this, the guys at the shop agreed they can implement this but when the parts are transferred to a similar machine that's a bit newer. Still seems a bit of a mystery but it will soon be a non-issue.

    Thanks everyone,
    BB

  20. #20
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    Why will it be a non-issue? Because of the newer machine? You should be able to do this on most of any machine providing that you have the right options on it.

    Stevo
    (The opinions in this post are my own and not those of machinetoolhelp.com and its management)

  21. #21
    Join Date
    Sep 2010
    Posts
    14
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Entering and managing tool offsets on a Dahlih MCV-760 w/ Fanuc control

    I'll try and explain this as best I can when I talk to you but basically you're correct, because the parts are moving onto a new machine. There apparently are the other offsets available on the existing machine but they have been told "not to use them" (that would take too long to explain in this forum!).

    BB

Similar Threads

  1. Niigata HN50C Fanuc 15M control, tool change arm
    By mach_repair in forum Machine Repair & Troubleshooting
    Replies: 0
    Last Post: 10-13-15, 11:39 AM
  2. A61 Makino Pro 5 control how to download tool offsets
    By cncfrank in forum Machine Repair & Troubleshooting
    Replies: 1
    Last Post: 02-13-13, 08:43 PM
  3. tool offsets
    By krueg57 in forum Programming / Applications
    Replies: 4
    Last Post: 08-31-11, 02:35 PM
  4. MagnaTurn South Bend Lathe Set Tool Offsets
    By badCAD in forum Programming / Applications
    Replies: 0
    Last Post: 05-23-11, 01:22 PM
  5. ABC offsets for fanuc and height/radius offsets for a mitsubishi
    By Anthony Magnolia in forum Machine Repair & Troubleshooting
    Replies: 0
    Last Post: 10-05-07, 03:45 PM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •