Touching tools off 2-4-6 block

[bjhall06]

Let me start by saying that I am accustom to Fanuc contollers and HAAS controllers are greek to me.

The school I'm attending has just acquired a HAAS mini mill and lathe. At the machine shop I work at, we touch all tools for production jobs off of a 2-4-6 block.

I set this up by touching the spindle off of the 6" block, then setting the relative Z positon to zero.

I then touch the spindle off of the top of the part and set my G54 (or other location) Z offset to zero.

I have talked to my instructor about this idea and he is very interested in doing it because of the multiple programs that this machine is setup to run.

Well I attemped to do this for him and I am completely stumped on how to set the relative Z to zero. From what I understand the "work position" is the same as a relative which is what is read to determine the Z location in a program.

I have jogged the spindle down to the top of a 6" block and I can not figure out for the life of me how to set this Z postion to zero. Can anyone point me in the right direction?

[CNCRim]

On the Haas, after touch off 6" block go to Work postion page highlight Z hit origin(F4), then bring the tool up/down touch top of the part. The Z on the screen is your Z relate. For Fanuc, go to Relative Position hit Z0 input, repeat same process.

[-Chris-]

Hi, I don't know if this will shed any light on your procedure or not this is how i set up the 2 VF 4's i run daily. I first load tools in holders with enough stick out for max z depth tool will be cutting. Tools are then loaded into turret and all tool length offsets are made by touching off to the 2 inch side of 123 block setting on the table. When part is to be cut in a vice i usually do the setup with part replaced by a 123 block on parallels in vice pushed up to stop. I'll Set first tool offset G54 with edge finder for my x & Y Zero's. I'll load a tool usually a end mill that is making a critical depth cut like a blind pocket into the spindle and jog it down to the surface of the 123 block and a .250 standard i have.At this point i go to the offset pages to the tool in the spindle and subtract the current Z location (bottom left of screen) from tool length offset value for tool in spindle. This number is then placed in g54 Z register. so now my z is set to 1.250 above parallels so i just type -1.25 hit write/enter and it will adjust g54 Z value down 1.25 so now my z is set to top of parallels. now say my stock is 3.00 tall i add 3.00 to g54 z to raise it above parallels 3. inches. offset is done and all the offsets are the same.
I guess maybe what I'm getting at is there are as many ways to setup a cnc as people running them. This works great for me -Chris-

[bjhall06]

Originally Posted by CNCRim On the Haas, after touch off 6" block go to Work postion page highlight Z hit origin(F4), then bring the tool up/down touch top of the part. The Z on the screen is your Z relate. For Fanuc, go to Relative Position hit Z0 input, repeat same process.

This is what I was trying but the position would never change to zero. I was in jog from where I moved the spindle down to the top of the block. Then I pressed Z which in return made "Z" on the Work Coordinate Position flash. Next I pressed Origin and nothing happened. Am I missing something?

[CNCRim]

That's strange, try Z0 write. Did you try bring up diffrence page and try see if Z is zero out?

[bjhall06]

Yea I tried everything i could think of..

Z0., origin; Z0 origin; Z0 alter, etc.

The display I was on was Posit, Page down (to "work") then "Z", then "origin".

But nothing changes when i do this. On Fanuc controllers the Z number will always set to 0 or whatever you want to preset it to.

It is a mini mill, but I dont know what that would matter. It seems like all HAAS controllers are very similar.

[tnik]

the "work" page is the value from your G59 (or whatever) work offset to machine zero.. You want the operator position page to be able to origin (zero) out your axis.

[FastIndy]

Usually what I do is touch off every tool to the 1" side of a 1-2-3. Then I pop the dial test indicator into a chuck, and dial the same face of the 1-2-3 in to a value I'll remember, like a nice even 10. Then I'll zero the operator coordinates by making sure I'm in the position page, entering "Z0.0" and pushing ORIGIN. Then I'll move the table and run in the same number on my dial indicator on the surface of the part, top of the parallels, or whatever. When my dial indicator is reading 10, the operator Z coordinate is at the proper Z offset so I just read that value and key it into the G54 Z offset. That way you can set all your tools once for any setup you're going to run, and dialing in the Z zero takes about 1/10 the time it took for me to write this paragraph - usually around 30s if the dial indicator isn't in a chuck.

For the Machine Offsets...First, you have to make sure that the G54 (or whatever origin you're using) Z is highlighted in the Offset page. If you push the "Part Zero Set" it will zero Z at the current position. If you key in a number like "5.1440" (note, no Z) and hit F1 it will change Z to that value, and if you key in "5.1440" then enter, it will add 5.1440 to whatever value is already in the Z register. If you push ORIGIN while you're here, it will zero ALL AXIS for that coordinate system.

Like tnik said, to temporarily zero out your axis (at least on newer controllers), you need to hit POSIT to enter the operator position page.

Nate

[bjhall06]

I got it working yesterday. I ran a program and everything worked out. I only ran into one issue, which isn't a big deal and I can work around, but more of an inconvenience than anything.

When a program reads the height of a tool it is based on the "operator position in the Z axis". So when I touched each tool off of the 2-4-6 block and press "tool offset measure" it inputs the "machine position" instead of the "operator position" which results in a negative (-) number instead of a positive which it should be.

Is there a way that when I press tool offset measure that it inputs the operator position like it should? Is this just a parameter issue??

To work around this, I just manually put in the operator Z axis position instead of using the "tool offset measure" button.

[-Chris-]

From what i take away from the HAAS manual and all my experiences on our CNC's Haas's standard way of setting up a job is to set all tool lengths to the top of your part stock and also set your fixture Z offset to the top of part also. This would make all cuts into the stock a negative value. According to our manual and quick start guide it says to only use PART ZERO SET for X & Y in your Fixture offset and have Z set to zero on the setting page for say g54. change it there don't use part zero set for z values.Also know that when you set tool lengths from another location than top part the z value will be the difference between where you touched off your tools and and your Fixture offset Z value -Chris-

[lkenney]

Here is how I set up my Haas.
1. I use a 2" high block with a dial indicator in it, you can buy them or make them. I set this block on the rear left corner of my right hand vise just to be consistent.
2. I touch off every tool to zero to the 0.0001" on that block.
3. I place a piece of material in the vise or softjaws as we will for production work. I change tools to an endmill (usually tool 6 which is my standard 1/2" end Mill) and locate it over the top of the materials, usually over a area that will be cut away.
4. I lower the endmill to close to the material and turn the spindle on usually at about 1000 rpm. then I gently lower the end mill to where it just starts to touch the material, should leave a thin circle line cut on top of the material. I stop the spindle, open the offset page and go to that tool position (T6).
5. On the bottom of the screen is to tool z axis location where it is touching the material. I subtract this position from the tool zero and key that into the G58 or what ever work Zero I will be using.
6. If the material is taller than your 2" offset block the Z axis zero will be a positive number, if it is lower than the 2" block it will be a negative number.
7. Now all the tools are zeroed to the work piece. If you break a tool or wear one out, Just rezero it with the indicator block to whatever 0.0001" and you are ready to go.
8. I try to always use a known point like the right front corner of my rear, fixed vise jaw and use that for my X and Y zeros.
9. It takes longer to write about it than it does to do it. If I change operations to a new piece or a different side of the work piece, give it a different operation Zero like G56 or G114 use the same steps to set the work height for the new work zero and carry on.
10. I usually use g54 through g59 for my right hand vise and G110 on to G?? for my left vise. It is just an aid so that I know when I read a program 6 months from now what vise I set up on.


Good Luck, Have fun and make Swarf
Lowell