H#107 ???

[springer82]

Hi Everyone,

I am doing a program that will pick one of 5 drills and reamers. I am almost done. Only one more problem to deal with. I have set my program to pick the right drill and reamer. When it comes to the TLO I am having a problem.
We set our tools off a 2" touch off block from the table of the machine. All tool lengths are "negative". In normal G code programming this is not a problem. Now using H#107 as a call it is a problem. I have used G43 and G44 with no luck. ??????? I get a #006 alarm. "Illegal use of negative sign". Sign "." input error,, sign "-" was input after an address with which it cannot be used. Or two or more "-" signs were input. I set #107 from #10003. I see when it goes into #107 it has a few "0" in front of the number (#107=-0013.5286). Can this be a problem?? I do not understand why there is a problem setting the H. Can some one put me on the right path!! Thanks for your time.

[beege]

Let's see,

If you program G43 H1, you get an offset from offset #1 in the table, which will affect your tool length by a negative value. If you program G43 H-1, the control doesn't know what to do with that negative number, because -1 isn't a spot in the table. You don't program the H with a direct numerical value. If needed to use the offset value from the table, you'd use it directly, without the G43 or G44, as in: Z[0+#107]. Any clearer?

[stevo1]

What model control are you using this on?

Having a few 0 in front of the number should not matter. What matters is the placement of the . decimal.

Any chance you could post the code where the error is happening?

It sounds like Beege may be on the right path to your problem but without seeing the code we can only speculate.

Also what is alarm #006? Is there any prefix to the alarm like PS, EX, etc?

Stevo

[psychomill]

I'm with Beege and Steve seperately... Got part of the problem idea.....
Here's what I see....


Your problem is this:

If #107 = -13.5286 and you use this:
G43H#107

You just told the machine to use height offset number "-13.5286". If you can find that offset number (tool number, pocket number, etc) then you would be good but you're not going to find it.

G43 reads from the offset tables meaning a variable string (H in this case) needs to be a valid number you have on the tool offset table which is a whole number (1, 2, 3, 25, etc). In otherwords, "H#107 needs to be able to look up a number on the offset page (#107=1, #107=2, etc...).

You do have a tool offset page right? (If you're pulling from #10003 then you have at least 3 tool offsets!) You can skip all this just simply by putting your tool offsets right to the offset page and then using straight H calls like G43H1, G43H10, G43H6.......

[sinha_nsit]

Therefore, have -13.5286 in H-geometry column of row number 3 (for example), and command G43 H03.

#10000 and #11000 series can be either for geometry or for wear offset, depending on parameter 6000#3.

[stevo1]

Wow…ok it is plain as day now. You are correct Psycho that is the problem. Can’t believe that I missed that last night

Didn’t you know that all the new machines are coming standard with 13.5286 in the tool offset tables?

Stevo

[springer82]

Hi Everyone,
I would like to start by telling you that H3 and #10003 hold the same numbers. That would be "-13.5286". As for controls I have a Fanuc 16i-M on a Kitty with 30 pods. Beege,,, I had hopes for the arithmetic way you posted. SORRY.. all I get is alarm #006. I tried many different way to do it too. Still no good. I posted the alarm on my first post. Here it is again: alarm #006= "Illegal use of negative sign". Sign "." input error,, sign "-" was input after an address with which it cannot be used. Or two or more "-" signs were input". That is straight out of the manual. Here is the code from the drill.

(#100=27 FOR SMALL POSTS)
(#100=28 FOR LARGE POSTS)

(#101=1 FOR .0952 I/D)
(#101=2 FOR .1157 I/D)
(#101=3 FOR .1383 I/D)
(#101=4 FOR .1540 I/D)
(#101=5 FOR .1792 I/D)


#100=28 (POST SIZE)
#101=5 (I/D SIZE)

(TOOL LENGTH FOR DRILLS)
N5IF[#101NE1.]GOTO6
#107=#10003
GOTO20
N6IF[#101NE2.]GOTO7
#107=#10011
GOTO20
N7IF[#101NE3.]GOTO8
#107=#10012
GOTO20
N8IF[#101NE4.]GOTO9
#107=#10013
GOTO20
N9IF[#101NE5.]GOTO9900
#107=#10014

( OPERATION 3 HOLES )
( RGH DRILL FOR REAMER)
N300
G0G17G40G49G98G90G80
S1800M3
G90G54G0X-1.55Y-.19
T4M106
G43Z.35H#107M8
Z.1

Now,, here is my question. Because H3 and #10003 are the same,, and they are both "-" what is the problem. I look at the tool page like a spreed sheet that the machine company give us as easy access to the variable page. Yes you can change the numbers on the tool page but they are stored in a separate variable. For me it is H3 and #10003. I might be way out in left field. ??? That is why I am here. In standard G code programming I use "-" numbers all day every day. The tool page is ALL "-" numbers. That is the way it is. When I program "G43 Z.1 H3" it is calling a "-" number. When I program "G43 Z.1 H#107" it is calling a "-" number. The same number. I have tried H#107, H[#107], H[0+#107] and, and,,,,, In macro programming this should not be a problem. I'm sure it is a simple fix that is right in front of me. I just can not see it. I still think part of the problem is in the way #10003 sets itself as -0013.5286. I know from reading sinha's book sometimes you have to change a parameter to get things to work???? Maybe?????? Once again,,, Thanks for all your help!!! ;-)

[chucker]

not sure if I grasp what your doing but heres a shot at it. call your tool change and your H some thing like I have it and leave it out in the lower part of your program




(TOOL LENGTH FOR DRILLS)
N5IF[#101NE1.]GOTO6
T1M6 (ADD TOOL CHANGE)
H1 (Delete the #107=#10003)
GOTO20
N6IF[#101NE2.]GOTO7
T2M6
H2
GOTO20
N7IF[#101NE3.]GOTO8
T3M6
H3
GOTO20
N8IF[#101NE4.]GOTO9
T4M6
H4
GOTO20
N9IF[#101NE5.]GOTO9900


( OPERATION 3 HOLES )
( RGH DRILL FOR REAMER)
N20
G0G17G40G49G98G90G80
S1800M3
G90G54G0X-1.55Y-.19
G43Z.35M8 (LEAVE OUT THE H)
Z.1

[stevo1]

Yes it is a simple problem right in front of you. As Psycho has already stated there is a difference between what you are setting.

When you use G43H3 it is “looking” for a value in the table under tool 3, it is not setting G43H-0013.5286. It does not care what that value is. If you were to program G43H7 it is “looking” for the value under tool 7.

So when you program G43H#107 it is actually G43H-0013.5286 and it is looking for tool number -0013.5286 which is “not” in your tool table.

You can only use a value in the H() that is in your tool table ex 1-? however many tools you have. If you need to offset by the value of tool 1 you need to program H1. If you want to offset by the value in tool 10 you need to program H10.

Stevo

[springer82]

Originally Posted by stevo1 Yes it is a simple problem right in front of you. As Psycho has already stated there is a difference between what you are setting. So when you program G43H#107 it is actually G43H-0013.5286 and it is looking for tool number -0013.5286 which is “not” in your tool table. Stevo

This answer sounds more reasonable. I still think that G43H#7 is the same as G43H3. They are both -13.5286. BUT,,, if in fact it is looking for tool number -13.5286,,, then it is a lost cause. If the "H" designation starts more then just calling up a number then I need to find a different way to do this.
Thanks for your help. And rewording.

[stevo1]

For the sake of having to reread, what exactly are you trying to do?

I understand the philosophy of what you are trying to do but not the reasoning behind it. I do the same thing in all of my tool change macro programs. I use G43H#20. This ensures that I am using the current tool that is in the spindle.

I think you are looking at this too much. When G43 is used it needs to know what offset value to grab. So you have to tell it where to look for the offset value. If you tell it H3 it is going to look at the value in tool 3 offset table it is not setting H=-0013.5286.

So with all of that said if you put the proper offset value for tool 3 in the offset table as you have -0013.5286 and then program G43H3 your offset is active and you are good to go. If you are trying to use a variable to accomplish this then you have to set the variable to 3 not to the value of what is in tool 3. So #107=3. Mod your program like so.

(TOOL LENGTH FOR DRILLS)
N5IF[#101NE1.]GOTO6
#107=3
GOTO20
N6IF[#101NE2.]GOTO7
#107=11
GOTO20
N7IF[#101NE3.]GOTO8
#107=12
GOTO20
N8IF[#101NE4.]GOTO9
#107=13
GOTO20
N9IF[#101NE5.]GOTO9900
#107=14

I hope this helps.
Forget answering my first question as I now see what you are trying to do.

Stevo

[psychomill]

I still think that G43H#7 is the same as G43H3. They are both -13.5286.

No, they are not.

Bottomline, your thought process is saying this:
G43 H-13.5286

That is not a valid command