Haas Mini Mill - Part locate

[JAMMAN]

Hi all,

 

Just bought a Haas mini mill and it has to be one of the easiest controllers to navigate I have ever played with.

 

We have been making parts since the 4th day it was in the building, but there has to be an easier way to pick up the top of part than setting all the tools at the top every part.

 

All I want to do is set the tools once and use G54 for the Z also.

 

I bought one of those fancy electronic feeler gadgets and I have a height indicator too.

 

T1 is the feeler. If I set all my tool offsets to 2" above table, put the offset of the feeler to 2" above the table, I still can't make any sense of the number I get with T1 in the spindle when I touch top of part. It puts a negative in G54Z and it should be a positive. It will not let me enter a positive number for T1 offset to fool it.

 

So from the guru's corner here at e-mastercam....

 

How do you locate your parts?

[bet338]

Jamman,

Z workoffsets are a negative number on haas's.

Don't know why they are but I program 11 of them here and that's they are setup. Completely opposite of our two Kitamura's

HTH

[NeilJ]

I'm no Haas expert but maybe check parameter 64.

 

"This setting changes the way the Tool Offset Measure button works. When this is ON, the entered tool offset will be the measured tool offset plus the work coordinate offset (Z axis). When it is OFF, the tool offset equals the Z machine position."

[JAMMAN]

Thanks bet and Neil.

 

So bet.... how do you or your operators pick up the part top?

[Metalmuncher]

On our Haas we set all tools off the table, then measure the distance from the top of the part to the table, it will be a negative number but you have to make it a positive number. Z "0" is the table top any negative number is below the table top.

HTH

[JAMMAN]

Wow that's my worse fear Mr. Muncher. I really really want to touch the top of the part with my probe and press a button.

 

This would be avoided if I could enter a positive value in the tool offset for T1 to fool everything.

[Guest]

Measure the distance from the face of your spindle to the table.

 

That value will be your G54 Z offset, it should be plugged in as a negative value.

 

The measure the distance from the table to the top of your part, enter that as your TLO as a + value.

[J Coulston]

I locate almost all of my parts from Z bottom. Before tool setters I used a 2" electronic height gauge. Y

 

You need a place on the table or vise that will never change and will always be accessible. I measured the TLO from that position adding the height of the gauge.

 

I use a lot of step jaws. I always used a work offset G54P48 that contained the difference between the location of the electronic gauge and the top of my step jaws to set my tools from. With the calculations set in the background I just have to enter the work offset from the top of the jaw ie. .100 jaws Z-0.1, .490 jaw Z-.490. If I am profiling around a carrier I use Z0.02 on the machine work offset, in MC I profile a at Z-0.01, I know that I am not going to hit the jaw.

Another benefit of setting tools this way is If I have to calculate a height of a part I can place the gauge on top of the part, activate the work offset and the spindle tool TLO, handle down till the gauge lights then adjust the work offset so absolute to read Z part value plus 2.000.

 

I the feeler gadget is and XYZ electronic you could set the TLO from you electronic 2". Then activate T1 and the work offset you want to set Z. Handle down and adjust the Z to read whatever your Z part value is.

 

You do not need a reference tool with this method. All the tools are set relative to one another.

 

 

Hope this makes sense.

[NeilJ]

We touch the tool height offset gage and set the dial indicator to zero and then we zero out the Distance To Go in the Haas control.

 

Then we touch the top of the part until we zero the dial indicator and enter the number that Distance To Go now displays in the fixture offset (G54, etc.)

 

If the part is below the tool height offset gage you get a negative Z number. If the part is higher than the tool offset gage you get a positive Z number.

[JAMMAN]

The work arounds are cool. I've been playing all morning here's what I see-

 

Set all tools with the 2" height indicator off table.

 

Set tool height of T1 (feeler) to a 2" jo blok off table.

 

Write down the number of the tool length of T1.

 

With g54Z at zero, touch top of part with feeler.

 

Whatever is in Z, subtract it from the length (as if both numbers were positive which they are not) and enter the result as a positive value in G54Z.

 

Man why is this so difficult? Is there a way during jog mode to get it to read the tool offset as if it was in a program?

[Greg_J]

The way we do it is that we measure the exact length of the tool from the spindle nose to the tip of the tool. That positive value gets put into the tool length offset for each tool. Then for each part I do I use a touch off sensor and I touch my spindle nose to that sensor and then move in the value of the sensor then that is my Z value for that work offset. I don't have a probing system or touch setter for that machine.

 

My .02$.

[Gary]

We do it like you jammer exactly but I keep the tool 1 (probe) number on a piece of paper at control. Now I use tool 1 to touch top of part. I type in the wrote down offset and hit f1 to enter it absolutely I then type in the number on the bottom of offset page (machine position) and hit the right enter button. It does the math for you. It even takes into account the pos/neg numbers when typed in. I touch all the tools of the 2in block on the table and use the tool offset button to set them. I keep the pad in the corner of the table and set g59 to center of pad. Its then mdi g59 x0 y0 and touch top of pad.

[JAMMAN]

Hmmmm didn't know about the F1 trick, I'll have to try it out monday when I'm back at it.

 

So F1 enters it without "adding" it to current value?

[NeilJ]

F1 overwrites whatever the value is and replaces it with the value you entered.

[JAMMAN]

Dang that already saves me all kinds of time and I haven't done it yet. I really don't know of any use for the adding thing it does when you just enter a number using that lower right hand button whatever it says.

 

You have to understand I've run about a dozen different controllers but this is the first Haas. Love it so far, learning every day.

[67 Yankee]

The way I like to set part and tool heights on my Haas machines is to set all tools with a 4" tall setter sitting 6" above the table on a 2-4-6 block. We may not need to have the tool plane that high, but it prevented some problems back in our Fadal days and we didn't need to change the method when all the Fadals went away.

When the tools are set, we'll typically pick any tool that's convenient for setting the part height, run the tool down to touch the top of the raw stock, then move off the part and drop another .02" or so to clean up the stock. hit "offsets", put the cursor on Z and hit "part zero set". That will enter the current machine position into your offset. Then hit the page up button and look at the length offset for the tool in the spindle. The offsets will be negative, and we just type in that number positive instead of negative, page up again to get back to your part Z and hit enter. That adds the tool length back in to the G54 offset without having to write anything down and no chance of math errors. Sounds like a lot to write out, but if you try it, you'll see that it's very quick and simple.

[EazyE]

I set up haas machines all day - the ones without probes there is only one way to go - I have a 3" post mounted to the table. Using a 123 block jog the spindle down to touch. (pick a offset that will never be used for anything else) cursor on z value for this offset and part zero set(minus the side of 123 block used) now use this offset to set all tools all the time. (i have a prog that moves table to post and loads g129 )... Once tools are set. jog to top of part and set z. Now every time u need to add a tool just make sure you are using g129(or what you choose)and touch off at post. With this method there are more options to adjusting your work. If any tool is cutting + / - you can simply change it in the value for the tool. If the part is + / - height then just change the z for the offset....

[X-L Engineering Corp]

We use the method John had explained earlier.

_______________________________________________________________________

Measure the distance from the face of your spindle to the table.

 

That value will be your G54 Z offset, it should be plugged in as a negative value.

________________________________________________________________________

The only difference is we don't use the TLO I have my Operators set the tools outside the Machine using an extra tightening fixture on a surface plate with a height stand.

 

Zero on top of tightening fixture like it's the face of the Spindle and measure to the top of the tool then enter that positive number in your offset registry.

For a fixture or Vise measure the distance from the table to the top of your part, use that number to subtract from the G54 "Z".

And for an indexing head just subtract the center height difference in G54 "Z".

And now you don't touch off tools in the Machine everything is done off line, It's a vary cheap tool pre-setter that works great.

[JAMMAN]

I can't get the tool registry to take a positive number for an offset.

 

I bought one of those fixtures that nests the cat to possibly measure height on a surface plate. Love it but still coining a "method"

 

 

Hey thanks by the way for all the responses, I'm learning a lot.

[Tony35]

to enter a positive offset you need to go into settings and change it to positive offset

HTH

[NeilJ]

quote:

---

I can't get the tool registry to take a positive number for an offset.

---

Did you try what I posted to you earlier in this thread?

 

Check parameter 64.

 

"This setting changes the way the Tool Offset Measure button works. When this is ON, the entered tool offset will be the measured tool offset plus the work coordinate offset (Z axis). When it is OFF, the tool offset equals the Z machine position."

[JAMMAN]

Parts are running and will be till next weekend before I can "play" again but it looks like you can enter anything you want with F1 which is a blessing.

 

I do need to set parameter 64 to off because it is now on, I'm assuming this because it does currently take G54 in to account when setting offset lengths.

 

Jim