Need Help!- Set Up Opionions Wanted

[LockTech]

Recently we upgraded from a non ATC PC-based CNC mill to a 2011 HAAS to improve production. This was a huge upgrade as you can imagine and is coming with quite a learning curve as well.

It will be used for production work with a number of different (but very similar) fixtures. With the switch over to the HAAS I want to remake the fixtures and as I have learned on the table top mill making fixtures the same dimensions for zeroing xyz is a huge time saver when switching from fixture to fixture.

I realize this is a loaded question with many different options, but thats what I wanted....opinions.

My main concerns are whats the best way to setup the z axis using the ATC for the way I will be using the HAAS? Each fixture will require approx 5 tool changes before needing to be swapped out or reloaded.

Having an ATC and very little knowledge of my HAAS still I am faced with whats the best way to get the bits to a known height in the carousel? And the best way to get them zeroed on the work piece. I have coming in the mail a Haiger Zero Master when I am really looking forward to and want to leave in place in the ATC.

My main concrn at the moment is doing the fixtures right using the ATC because I dont want to have to remake fixtures later down the road.


TIA

[Geof]

Don't worry about trying to design your fixtures to any preconceived dimensions to try and match tooling lengths. There are several ways to adjust the Z offset when a fixture is changed. I think most people would suggest having the probe option on the machine. My place does not have probes on any machines so we do it the 'hard' way which is quite simple. Have a reference point independent of the fixture which you use for setting the Z offsets, we make it higher than the highest point on any fixture. Then in the program(s) associated with each fixture have a G52 Z command that adjusts for the distance between the reference point and the fixture.

[TXFred]

Here's one way that I am a fan of.

Set tool 1 to 0 length.
Measure tool 1. (We have a height gauge and fixture for this.)
Zero the height gauge.
Measure tool 2. Enter the value on the height gauge into the offset for tool 2. If tool 2 is shorter than tool 1, you will have a negative number. If Tool 2 is longer, you will have a positive number.

Repeat for the remaining tools.

Next, you need to locate your origin. Position Tool 1 at your part's origin.
Use "Part Zero Set" to fill in the G54 X, Y and Z offsets.

You're ready to run.

If you need to change a tool, you can easily change it and correct its offset by the same method.

I like this method because it has a good reality check built in. On the Tool offset's page, if Tool 2 has an offset of -2.5, then tool 2 should be 2.5" shorter than Tool 1. That's easy to verify visually with the tools in the carousel.

I've attached a picture of the fixture that we use. When I'm setting up, I just take this to the machine so I can quickly set all the tools.

[TXFred]

Here's the other way that I use for quick setups that only use a couple of tools. It's not as precise, but it's faster.

Under G54, leave the Z offset at 0. Enter X and Y the way you normally would.

Select Tool 1. Jog the machine in -z until the tool is close to the work.

Slide a Post-It note between the tool and work, and jog down in 0.001" increments until the paper is pinched. Jog up 0.001" to release the paper. Jog down 0.004" (Thickness of a Post-It note).

Go to Tool Offsets, select the offset for Tool 1, and hit "Tool Offset Measure."

Repeat for the remaining tools.

Stick the Post-It note to the side of the mill's console, and if anyone asks, tell them that it is ISO9000 Calibrated Paper.

Frederic

[awilliams684]

Originally Posted by TXFred Here's one way that I am a fan of. Set tool 1 to 0 length. Measure tool 1. (We have a height gauge and fixture for this.) Zero the height gauge. Measure tool 2. Enter the value on the height gauge into the offset for tool 2. If tool 2 is shorter than tool 1, you will have a negative number. If Tool 2 is longer, you will have a positive number. Repeat for the remaining tools. Next, you need to locate your origin. Position Tool 1 at your part's origin. Use "Part Zero Set" to fill in the G54 X, Y and Z offsets. You're ready to run. If you need to change a tool, you can easily change it and correct its offset by the same method. I like this method because it has a good reality check built in. On the Tool offset's page, if Tool 2 has an offset of -2.5, then tool 2 should be 2.5" shorter than Tool 1. That's easy to verify visually with the tools in the carousel. I've attached a picture of the fixture that we use. When I'm setting up, I just take this to the machine so I can quickly set all the tools.

My setup looks a lot like that, same height gauge. I made a holder similar to this to hold my tooling for measuring.

[Geof]

Originally Posted by TXFred Here's the other way that I use for quick setups that only use a couple of tools. It's not as precise, but it's faster...... ......Stick the Post-It note to the side of the mill's console, and if anyone asks, tell them that it is ISO9000 Calibrated Paper. Frederic

It is astounding how repeatable paper thickness is. With a sensitive touch you will get the same precision as your height gauge.

[TXFred]

Originally Posted by awilliams684 My setup looks a lot like that, same height gauge. I made a holder similar to this to hold my tooling for measuring.

Do you get accuracy with that holder? It doesn't seat against the taper, and I would expect some variation in the height of the collar on the tool holders.

Frederic

[LockTech]

Geof, that makes sense, do you ever run into an issue with wanting to mill something higher than your originally set "high" point?

Frederic, would there be any reason to make the tool being measured at 0 not be the probe? It seems like that would make it more of a permanent baseline as bits get replaced for various reasons? Also does it need to be tool1? the reason I ask is that it seems to want to keep tool1 in the spindle. Any advntages/disadvantages to have tool1 be the probe?

[TXFred]

Originally Posted by LockTech Frederic, would there be any reason to make the tool being measured at 0 not be the probe? It seems like that would make it more of a permanent baseline as bits get replaced for various reasons? Also does it need to be tool1? the reason I ask is that it seems to want to keep tool1 in the spindle. Any advntages/disadvantages to have tool1 be the probe?

It makes perfect sense to have the probe be the 0 length tool.
The reason I don't do that is that none of the mills here have a probe.

It can be any tool you want, so long as you use that tool for all your touching off. (Having typed that, I now think it sounds obscene.)

Frederic

[Geof]

On our production machines we never need to go above the 'high' point.

When I am doing prototypes and tooling I either use the paper method directly on the part or I make a temporary high point using a 2,4,6 block.

Here is a thread I started years ago which goes over setting Z offsets quite well.

http://www.cnczone.com/forums/haas_m...sets_mill.html

[awilliams684]

Originally Posted by TXFred Do you get accuracy with that holder? It doesn't seat against the taper, and I would expect some variation in the height of the collar on the tool holders. Frederic

Im using the backside of the flange on the tool holders for reference, probably not as accurate as going off the taper as you stated, but it has given me good results. Usually as long as im not in too much of a rush its withing about 5 tenths. Im also using a lot of the same tool holders, so that could be a reason the deviation isnt that noticeable.

[LockTech]

Thanks, that helps alot on clearing things up in my head.

Didnt really sound obscene until I reread it lol