| scott |
|
|
Reply with quote | #1 |
today I was setting up a puma 230 with a fanuc 21t control...I tried to use a g10 p0 z-? command that I use often on other machines, and it didn't work. There was no alarm or anything, it read the line but did not change the workshift value. I know this is the correct address and format, as I use it all the time on other machines. Is there a parameter to enable g10? I looked in the manual and couldn't find anything.
Thanks.
|
| |
| Jeff |
|
|
Reply with quote | #2 |
Scott,
Try #2601=? the ? is the value you want to put in your Z workshift amount (just your value no letter)
Example: #2601=-10.00
This will change Z workshift value to -10.0
Try this in MDI should work.
Good Luck,
Jeff
|
| |
| Stevo1 |
|
|
Reply with quote | #3 |
I am really surprised that you don’t get a “format error” alarm. What other machine controls are you using that this works on? The problem that I see is that you don’t have an address of what to change. This is done with the “L” value. By seeing the P0 I assume that you are trying to shift the “common” work offset. The “L” address for this is L2. So you need to program G10L2P0Z-10. If you wanted to change G54-G59 these are designated as P1-P6. So if you wanted to shift the G55 coordinate you need to program G10L2P2Z-10. For a 21T control check 9102.0 for your G10 data setting option. Stevo |
| |
| scott |
|
|
Reply with quote | #4 |
thanks guys, I'll try both of those things. stevo...I understand what you mean about the "L", and I thought about that, but i double checked my other programs and it's just g10p0. I checked today and the other controls are two 18t's and one 21t, so it seems like it must be a parameter thing. |
| |
| Stevo1 |
|
|
Reply with quote | #5 |
Ok I did some reading up on the 16/18/21 controls. You are correct you do not need to use the “L” value with the G10. However if you do not use the “L” you are specifying the tool offsets to be changed. So what are you trying to shift your tool offsets or your work offsets?? If you were to program G10P3Z-5 your tool offset for tool #3 should be 5” (absolute). If it is not I would check to make sure that you have the G10 option installed. My guess would be you have the option because the control will usually throw and alarm like “improper G-Code”, or “No Option”. But this is not always the case. Another thing that you could check is make sure that you don’t have a Min and Max set in your parameters for how much you can adjust a tool length at any given time. Once again I would think it would throw an alarm if this was the case. One quick way to tell if you have G10 option is just program G10L2P2Z10. Look at your G55 work offset to see if it placed a value of 10 in the Z. I do know that this is the proper way to change your work coordinates. I can’t speak of the tool offsets as I never change them as you are doing. However according to the book you are doing it correctly. Out of curiosity why do you change the tool offset through the program? Why don’t you just shift your work coordinates of the part in Z? Sounds too easy to make a mistake and crash if you don’t change your tool length back to the proper length, via tool offset or G10. Stevo |
| |
| Curt B |
|
|
Reply with quote | #6 |
I believe it's good practice to include the L1 or L2 on the G10 line to distinguish whether the intent is to overwrite tool lengths or work offsets. Sending tool length data from the presetter to the control thru the G10 method can do wonders in reducing data entry mistakes.
Without the G10 option here's the variables to directly overwrite the registry values for work offsets:
| #5201 | COMMON X | | #5202 | COMMON Y | | #5203 | COMMON Z | | #5204 | COMMON W | | #5205 | COMMON B | | | | | #5221 | G54 X | | | #5222 | G54 Y | | | #5223 | G54 Z | | | #5224 | G54 W | | | #5225 | G54 B | | | | | | #5241 | G55 X | | | #5242 | G55 Y | | | #5243 | G55 Z | | | #5244 | G55 W | | | #5245 | G55 B | | | | | | #5261 | G56 X | | | #5262 | G56 Y | | | #5263 | G56 Z | | | #5264 | G56 W | | | #5265 | G56 B | | | | | | #5281 | G57 X | | | #5282 | G57 Y | | | #5283 | G57 Z | | | #5284 | G57 W | | | #5285 | G57 B | | | | | | #5301 | G58 X | | | #5302 | G58 Y | | | #5303 | G58 Z | | | #5304 | G58 W | | | #5305 | G58 B | | | | | | #5321 | G59 X | | | #5322 | G59 Y | | | #5323 | G59 Z | | | #5324 | G59 W | | | #5325 | G59 B | |
|
| |
| scott |
|
|
Reply with quote | #7 |
thanks guys for the replies...but just to clear things up...g10p0z-2. changes (or should change) the z WORKSHIFT...not the tool lengths. I have the g54-59 work coordinates, but that's not what I'm using to set my program zero. I have finally gotten the guys in the shop to use and understand workshift, so that is the way we set stuff up, I only use the other work coordinates on the mills. I have a program where I flip the part over to do both sides, so I had the g10p0z? line in the beginning for the first side, and then again after the m0 for the second side. Could it be that the Z value has to be positive? I'll see if I can mess with it tommorow. |
| |
| Stevo1 |
|
|
Reply with quote | #8 |
Ok when you say WORKSHIFT you are trying to change your common work offset No.00(common)? The reason you are seeing no change is because on your series control according to the book if you just program G10P0Z# with no “L” value it is going to your tool offset location and trying to change tool 0 but because there is no tool 0 nothing is going to change. Program a G10P1Z5 and look at tool 1 you will see that it changed to 5. Now if you are looking to change your work offset NO.00 you have to use a “L2” to specify the work offset locations. So you would program G10L2P0Z1. Now look at your common work offset and you will see 1” in your Z value. If you specify any one of these in your G10 line this is what it will change. P0=No.00(common) P1=No.01(G54) P2=No.02(G55) P3=No.03(G56) P4=No.04(G57) P5=No.05(G58) P6=No.06(G59) Stevo |
| |
| scott |
|
|
Reply with quote | #9 |
I'm sorry stevo but you are mistaken. For one, you understand that I'm on a lathe right? Workshift is not common "00". If you go to offset page and over arrow one or two times you'll see "work" this is where g54-59 are, over arrow again and you'll see "w.shift" this is the value I'm trying to change. It could not have been going to tool #1 because I'm using tool #1 and I would've noticed if I changed my length offset. You may be right about adding the "L2", if I was using the "00" work coordinate, but I'm not. What book are you referring to? I couldn't find any real explanations, or list of addresses for g10 in my operator's manual. |
| |
| Stevo1 |
|
|
Reply with quote | #10 |
Scott, Yes I do know that you are on a lathe. When I initially looked up the G10 I was looking in the 16,18 manual. I am use to using the manuals based on a 16,18,21 so I didn’t bother to look at the applicable models. My mistake. I also do not use “workshift” only the “workoffsets” that is why I wanted to clarify if you were referring to the workoffset common or not. I usually like to verify on an the control before posting but I don't have a 21T model with me at the moment to check this out on. I now looked at the 21/210-TB for lathes manual # B-62534E/02. According to this you are correct that with a G10P0Z# this should change your "workshift". So you say it does not change. Can you change anything via G10?? MDI a G10L2P1Z1 and look at the G54 “workoffset” to see if it placed a 1 in the Z column. This is the code needed for your machine to set the G54. If it did not change then you might not have the G10 data setting option in your control. You probably have the setting because usually the machine will throw an alarm like “Improper G-Code” if you try a G-code that is tied to an option that you don’t have but I have seen them not as well. Stevo |
| |
| Curt B |
|
|
Reply with quote | #11 |
Another thing to remember is that G10 recognizes G90/G91 mode. Therefore:
G90G10L2P0X0Y0Z0 will change common values to zero
But in default G91 mode after reset, etc.
G10L2P0X0Y0Z0 will add zero to the existing values resulting in no change.
Making sure machine is in G90 mode is a must to make sure new values overwrite what was there and not blend with them.
|
| |
| Joe |
|
|
Reply with quote | #12 |
SteveO, plese don't post fanuc option parameters on this Forum, lest the lawyers shut it down. |
| |
| scott | |
