Haas lathes presetter

[lowboy]

Hello gentlemen, I was woundering if any of the experienced Haas lathe users could answer a couple of questions:

1.When using the touch probe,and touching off a drill, do you just Key in the X offset of some neg number to get it to center line?

Can you sweep the ID tool holder in and calc that position as X0 in the G54? Will it screw up the presetter?(that way if you want it to go to center, you leave the X offset 0)

2.Is there a position you can set where the tool always rapids to for indexing, like a G30 in Fanuc?

Thanks for everybody's time!

[chris m]

lowboy, I don't have a Haas lathe but I'll just comment on what I do with our Okuma machines as it may be helpful [or not].

 

We don't use our touch-setter in the X axis on drills at all, when we initially set up the machine we indicated all of the turret positions with an ID holder and recorded the X values on a spreadsheet so that any time the guy sets up the machine he can just key in the offset value in the machine which puts drills on center at X0. without having to think about it at all. I never use a WOFS or work shift change in the X, so the TLO values for the X-axis generated by the setter are always correct. In addition, we use a Z shift in all of our programs so that the Z-axis TLO value for the same tool is the same regardless of where the program Z0 is within the machine.

 

As far as the index point, I'm not experienced with Haas lathes, but I have some recollection that Haas machines have an optional "2nd Home Position" or something like that which could possibly be used for this.

 

Please let me know what you find out about this since I like to know as much as I can about different machine tools.

 

C

[Dan@home]

We just hit F2 without using the touch probe. That should be your X center. Then you can tram it in, if it is off.

[MACHINEMASTERG]

we use our presetter only for turning or groving tools like chris said for our drills or tap positions we sweep the turret position and recorded that location this will not effect the setter and for our tool change we send it home first ..g28....

[Thee Dragracer1951]

I also only use the presetter in Z on my Haas.

On my Daewoo...X zero is 0.0 in the control. The toolholder dias are at X 0.0 at the center line of the spindle. Makes it easy that way.

[CNCGUY]

quote:

---

Is there a position you can set where the tool always rapids to for indexing, like a G30 in Fanuc?

---

Unfortunatley not. We do tool changes at G59, set up in the post. That way the operators can change it as needed - long drills, short drills, etc.

[kenfromlodi]

for indexing at a position just use "G53 X0 Z0"

change the z value to move the index position closer to the chuck. on our sl-30 I almost always use Z-10. which will bring it 10.0" closer to the chuck.

[CNCGUY]

Ken,

 

I decided not to go that route since it would require the operator to change it in several places. Using a W/C method allows them to change it once for all tool changes. We have this at the beginning and end of each operation. This was done in case the operator has jogged the turret close for an insert change. This will allow them to cycle start rather than manually jog the turret away from the work piece.

 

code:

---

N2

G00 G59 X0. Z0.

G54 G50 S3400

M42

G97 S888 M03

T202 (SL LL O.D. 35 DEG. .015 R)

M08

G00 X4.3036 Z-.6609

G96 S1000

G01 X4.2328 Z-.6256 F.004

X2.9908 Z-.0046

G02 X2.9688 Z0. R.0156

G01 X.9235

X-.04

M09

G00 G59 X0. Z0.

M01

---

[kenfromlodi]

"there is more than one way to skin a cat"

so sure I understand and it is essentially the same thing except for once the "G53 Z minus" has been set it will always be the same unless changed in the source. I have my post set so I can move the index position in my source, this way the operator will not have to set an extra work shift every time which is in the control and can be different from job to job.

 

Anyway you do it there is always the chance of clearance issues if it is not right and caution needs to be used.

[Reece L Gibson]

Thank you all for the reply's.

I am geting ready to try them out

[lowboy]

Thanks for the reply's

I have one more question, How do you Calibrate the presetter arm?

[CNCGUY]

For Z, there really is no calibration.

 

For X, (O.D and I.D. - no drill) there are settings. Sorry I cant be specific, Im not in front of the machine or have a book right now. Page through the settings and refer to the manual for the procedure.

 

Or check this from there website. HAAS Manual Caution - 8MB file.

 

HTH

[chris m]

Don't know about Haas but on Okumas we calibrate both axes by using a tool with good offsets. If you swing the arm down and go to the parameter page the 'sensor position' parameters are automatically displayed; if you touch the "good" tool off it calculates the setter position using the turret position and "good" tool offset value. I would hope it is also relatively easy in your machine.

 

C

[lowboy]

Thanks for the link!

[Bryan Johnson]

on a related subject. Any recomendations for quick method to sweep the ID tool holders?

 

I am using a mag base stuck to the spindle, and test indicator, but was thinking there might be a faster way. Maybe something you would chuck on?

[DavidSV]

The number for the 'F2' button is a parameter. The parameter is in encoder counts. You can sweep in your holder and get the X value. Once you know what it should be, you can hit the F2 button. If its way off you can go into the parameters and change the encoder count for spindle centerline until when you hit 'F2' it comes out right. The spindle centerline parameter is 254.

 

To change it, follow these steps.

Go to settings

Type 7 then the down key (goes to setting 7, parameter lock)

Turn parameter lock off.

Go to parameter page.

Type in 254 and the down key (goes to parameter 254)

Change the encoder count by like 50 (make note of original number)

Go to offset page and hit 'F2'. Make note of new X centerline dimension and compare it to what you want. After a few times you can figure out how many tenths one encoder count is on your machine. Dial it in from there until you get it so that when you hit 'F2' you get the X value for centerline.

Turn the parameter lock back on and you are done.

 

After that using a drill or tap you just set the tip on the tool presetter and then hit F2 for the X setup

 

As far as calibrating the X diameter of the tool presetter, you can touch off a tool and set it, then make a little program to turn a small part, say 2" dia. Measure the part and move the number in the setting. The number in the setting is the diameter of the probe, so if your part is say .0023 small, make the number in the parameter smaller by .0023. The parameters on my Haas are 59 for the OD and 60 for the ID. You can set the Z if you really want to, but it works like its suppost to if you leave it at 0.000, and the Z- at the probe width.

[chris m]

coaxial indicators are the way to go for sweeping tools. MSC, Enco, everybody sells them and they're pretty cheap. We made a couple of stepped aluminum bushings with diameters that are common for us to hold our coax so that we wouldn't need to change the chuck jaws all of the time if we needed to sweep something.

 

C MSC coax indicator

[tryon]

hose clamp and a surface indicator

[Bryan Johnson]

I like the hose clamp idea, but may go ahead and spring for the coax indicator. It would also be handy on the mill.

 

Thanks for in info.

[Reece L Gibson]

A lot of good ideas

[Don S at Barefoot CNC South]

On some lathes I used the pre setter on drills and taps, touch in X then put 1/2 the drill dia. in the offset.