Tool number question

[Larry Myers]

Hi All

I have a silly question. Why does my Sharp 2412 (with a 10 tool carousel) have dozens of numbers in the tool offset? Why not just 10? What the heck am I missing here?

Thanks in advance.

Larry

[chuck5121]

Some machines use different offset numbers for Radius Compensators than tool offset numbers. you can use different offset numbers to set up multiple jobs using the same tools, using different offset numbers. Just like you use G54 G55 G56 and so forth for different locations you use different Offset numbers.

[Larry Myers]

Thanks Chuck5121,

To be honest, I am not sure I follow: If a 0.5" diameter end mill is in the tool number 1 position, how can I use the nuber 1 tool for anything other than the offest that it is set for? Is there some coorelation betwen T1 in the offset table and T11? I am not sure that I am even clear on what I am asking

In other words, how is #11 (in the offset table) and up even used?

Thanks in advance!

Larry

[timlkallam]

Hello Larry

Say you want to contor the outside of a part , You want to go around the part twice rough cut and a finish cut .So you write 2 different toolpaths . Some programers do it this way , I'm to lazy I just write the finish toolpath and paste it twice and use 2 different D addresses.

T01M6(. 5 inch end mill)
G54 G90G0X0Y0
G43H1Z0
G1G41 X?Y? D1( D1 calls up the tool radius used for cutter comp . I'm going to lie to the machine and input D1 as .255 this will leave .005 stock on the part for finishing .
G40 X?Y?

Finish cut same program
G54 G0X0Y0
G43H1Z0
G1G41 X?Y? D11 ( This time I call up D11 witch i imput .250 for the tool radius this will finish the part to the correct size.
G40 X?Y?
G0Z6
M30
Hope this helps

[Larry Myers]

Hi Tim

Good to hear from you again. And again, thanks!

I followed what you did there in your example. It seems that #11 and up are for ONLY diameter compensation (D). Is that correct? Or can it be use also for the Z distance from the part being machined?

Lets say I have a manual indexing head in the machine. There is a part secured to it. I have set T1 to the top of that part and set my Z=0. Then I mill a slot in the top of my part.

Then I rotate the head 180. I want to mill another slot using the same end mill. This time, and because of the irregular shape of my part, my Z=0 is 1" higher than the first time.

I know I can figure this out mathmatically, however is there a way to use the additional tool offsets (those beyond 10) to compensate for that 1" difference in Z ?

Or am I all kinds of messed up in my thinking as usual?!!!

Thanks again,
Larry

[timlkallam]

[QUOTE=Larry Myers;814292]Hi Tim

Good to hear from you again. And again, thanks!

I followed what you did there in your example. It seems that #11 and up are for ONLY diameter compensation (D). Is that correct? Or can it be use also for the Z distance from the part being machined?

Yes for both ,kind off , Think off that page ONLY as hight offsets (H) and diameter offsets used for cutter comp. (D) The tool number in the carosel does not have to match the H or D offset number.
T01 does not have to use H1 you could use H3 Its just easy to remember and setup tool 1 uses height offset 1 .


Lets say I have a manual indexing head in the machine. There is a part secured to it. I have set T1 to the top of that part and set my Z=0. Then I mill a slot in the top of my part.

Then I rotate the head 180. I want to mill another slot using the same end mill. This time, and because of the irregular shape of my part, my Z=0 is 1" higher than the first time. You can call H 11

yes

I know I can figure this out mathmatically, however is there a way to use the additional tool offsets (those beyond 10) to compensate for that 1" difference in Z ?

yes

You got the perfect example . Your not changing tools your changing tool height offsets. You can call up tool 1 and use any H (hight offset) on your machine you can use H1 through H400 you don't have to use tool number 1 with height offset number 1.

When setting up the machine using tool 1 you set your to Z0
then rotate the part 180 dreg. and set tool 1 (same tool) to Z0
this time using tool 11,S offset


So in your program
T01 M6
G0 G90 X0 Y0
G43 H1 Z0 ( H1 is the correct height for the first slot.)
G1 X ?
G0 Z6
M00 ( ROTATE 180 DREG)
G0 G43 H11 Z0 ( Now you have called up a different hight offset and still using the same tool.)

Tim

[Larry Myers]

Hey Tim

I think I got it! Thanks

I was thinking that T1 was supposed to "match" H1. That is not the case, afterall. From what I think you are saying is that I can match any H value to a tool number.

In other words, I could have a H value for T1 (a 0.5" end mill) and assign another H value (mabe H11, for example) for the same T1 tool later on. This is as long as I use a G43 Hxx before I use it.

Wow, this just opened some doors for me, if I have it right!

Again, like many times in the past, thank you!

Larry