[chad123]

Hi all,

We have a Tl-1, have had it about 6 months and it mainly just gets used for little things here and there. I have to do a small run of parts and am in the process of building a gang tooling holder for it. I think I have this mostly figured out but have a question about work offsets.

I understand how to set the tool offsets on a one by one basis for a part but I can see how this would be a pain in the butt if you are using different stock lengths with different programs. Do you have to go and reset each tool offset every time you change what part you are making?

I was hoping that I could set a WORK offset and just change that and be good to go. I understand work offsets on the mill and maybe I am incorrect on how they work on the lathe.
I looked in the manual, but the lathe manual in my opinion is just about useless, especially when it comes to the tl-1.

Could someone please walk me through a simple gang tooling with work offsets setup? I think I am missing some part of the big picture.

Thanks!

Chad

[Geof]

Try doing a search or scan through the threads in the Haas forum. This was discussed a while back.

I use gang tooling frequently on a TL1 and also multiple work offsets so if you can't find the previous posts I can give some suggestions.


EDIT:

Found it

http://www.cnczone.com/forums/showthread.php?t=33866

[chad123]

Hi Geof, Thanks for that link, I read that thread a while ago and have been looking for it. I think I have the tool Tnn stuff figured out, we will see.

The thing that I don't understand is the work g55 offsets, and how that relates to to the tool offset. I will keep searching..

Thanks,

Chad

[Geof]

....The thing that I don't understand is the work g55 offsets, and how that relates to to the tool offset. I will keep searching..

Thanks,

Chad

The G5n work offsest simply moving everything by whatever is in the offset table.

The machine uses G54 by default and if you never put any values in the G54 line when you do your tool offsets they are taken from machine zero.

The X tool offset, X DIA MESUR, is (nearly) always the spindle centerline.

For the Z tool offset, Z FACE MESUR, some people use the face of the chuck but I prefer to use the end of the stock; actually I normally make it the finished end so my rough stock starts out a bit further than Z zero.

When there is no value in G54 both the X and Z values in the tool offset table are the distance from machine zero to the centerline for that tool or to the end of the part for that tool.

When there are values in the G54 work offset then the tool offsets are taken from this position. For instance if you entered tool offsets with noting in G54 then put a negative value in G54 Z you are going to finish up with the tool somewhere inside the chuck.

I never use anything in the X value for work offsets but often use Z values in G55, 56, etc., but not G54. This is when I am using a length of bar making small parts where I can have enough material out of the chuck to part off two or more pieces.

To do this I set the machine up and put the Z tool offsets in at the end of the stock. As I mentioned G54 stays at zero but in G55 I enter a Z -value equal to the length of the part plus the parting tool thickness plus a facing allowance; G56 gets twice this, G57 three times, etc.

The program I make into a subroutine which is called after the selection of work offsets. Something like this;

O00000
All the normal stuff
G54 M97 P1000
G55 M97 P1000
etc
etc
G54
M30

This machines all the parts stepping along the bar and then goes back to G54 and stops.

To simplify setups I enter the values for G55, 56, etc from the program using a G10 offset entry command. This makes the program;

O00000
All the normal stuff
G10 L2 P1 Z0. (Set G54 to 0.) Not essential
G10 L2 P2 Z-1.2 (Set G55 to Z-1.2)
G10 L2 P3 Z-2.4 (Set G56 to Z-2.4)
etc
G54 M97 P1000
G55 M97 P1000
etc
etc
G54
M30

There are other ways to do the same thing. Also sometimes there may be reasons why you want to use X values in the work offsets but I think this is enough to go on with.

[chad123]

Ok, That is what I was confused on. Thank you so much! it all is getting clearer now. Now I get the gist of it all and have a place to start..

Thanks

Chad

[Wiseco]

For my part, I use one of the jaws to setup my tools offsets. I take an 1/4"tool steel and I put it on the front of a jaw and I touch it with tools tips to setup my Z offsets of every tools. This way, I'm sure I'm setuping always the same way.

I always use the G54 for the work offset. I have a TL-2 so no really use to have 3-4 work offset or use another one.

I use the X work offset when tolerances are small. I put something like 0.01 and when the part is turned, I mesure it and I reajusted the X work offset to get to the final tolerance.