[mgb1974]

Finally got our OTS twin probe system setup in our VF-2 Haas Mill. Having problems actually using the tool setter.

We go to the WIPS screen on the control. Tool change till we have the tool in the spindle. Hit F2 to go to the input screen.

Here is a example of what we input in the F2 Screen.

Tool offset number- 6
Approx length-2.0 (is just the length of the tool sticking out of the holder???)
Approx Dia-1.0
Z Distance- 0.0 and also tried random 3.0 (not sure what to put in there)

We then hit cycle start and run through the cycle. The tool comes down on the probe and hits it and then comes up. A alarm message goes Probe Open.

The tool offset shows 2.0 which is the same as the Approx length that we are putting in.

What are we doing wrong? The manaul isnt much help.

Thanks
Matt

[Cory]

Finally got our OTS twin probe system setup in our VF-2 Haas Mill. Having problems actually using the tool setter.

We go to the WIPS screen on the control. Tool change till we have the tool in the spindle. Hit F2 to go to the input screen.

Here is a example of what we input in the F2 Screen.

Tool offset number- 6
Approx length-2.0 (is just the length of the tool sticking out of the holder???)
Approx Dia-1.0
Z Distance- 0.0 and also tried random 3.0 (not sure what to put in there)

We then hit cycle start and run through the cycle. The tool comes down on the probe and hits it and then comes up. A alarm message goes Probe Open.

The tool offset shows 2.0 which is the same as the Approx length that we are putting in.

What are we doing wrong? The manaul isnt much help.

Thanks
Matt

The length you want is from the top of the flange on your toolholder to the tip of the tool (ie: spindle face to tool tip).

I'm not sure what the z distance is. I have an 07 VF-1 with the wired TS27R and none of the tool probing fields I've seen ask for the height above the toolsetter.

[extanker59]

What you're describing sounds more like the calibration screen to me. I have a long cycle time so I can't look right now.
Did you call your HFO? Are add-on probes handled different than factory installed probes? We get to our tool/probe screens by pressing Edit, then "PRGRM CONVRS" three times. It'll show the VQC program options. Press F2 and scroll down to "Haas VQC probe..." and press enter. Scroll down to "Tool Setting", press enter, and then choose what you want to do.
I gather that you don't have those programs. Your HFO should be able to get them for you.

[mgb1974]

Thanks guys for responses. I mill is a 2007 model so I think they updated where the software is. The probe system came with the machine, we just never got it going till now.

Cory,

So every tool need to measure the length of the tool sticking out of the holder?

No this is not the calibration screen. I went through that before and now we are trying to use it.

Thanks again

[cadman@teluspla]

just as cory wrote
measure from the top of the V flange to tip of the tool
the tool length is a ball park # so your tool does not tag the measuring anvil on the tool setter to fast.
my VF4 does not ask for the Z length though.(2006 machine with TS27)
you can probably check your system by doing a manual tool length setting.
you will find that in the same menu

[Cory]

Thanks guys for responses. I mill is a 2007 model so I think they updated where the software is. The probe system came with the machine, we just never got it going till now.

Cory,

So every tool need to measure the length of the tool sticking out of the holder?

No this is not the calibration screen. I went through that before and now we are trying to use it.

Thanks again

My machine only asks for tool length on certain probing routines. The only one I can think off of the top of my head is auto length-rotating, and maybe auto length+diameter.

[pmurdock]

You know.. I got that tool setter probe as well, but recently had to take it off to machine a large plate.. haven't put it back on since! I still use the spindle probe for x,y measurements, but find it's sometimes quicker to just measure tools to a part, then to have to worry about remounting the tool presetter... Just my mileage.. I'll probably reinstall it later on, but it really chews into the size of your table once you add a rotary table, vise, tailstock and your part! <grin> Guess it's time for a VF-7..

cheers!
Paul

[cadman@teluspla]

Paul which side of your table is your tool setter usually setup on.
We mounted ours to the very far left it gives enough room for a 15" chuck
and 2 6" double lock vise

[mgb1974]

Got it figured out. Went into the VQC screen instead of the WIPS screen.

Question I have now, which i have struggled with since reading about the probes. How does the programming work relative to the tool lengths? Most of our tool lengths are set off the fixtures(program center X0 Y0 Z0). This usually gives us a negative number around -11 or -10 area. Now the numbers using the tool setter are positive(basically the length from the spindle gage line to the end of the tool)

Do you set your program Z0 Offset at 0 or do you set it at machine Z measurement(example of like -10.560)?

How does this work programming wise???

Thanks
Matt

[pmurdock]

Paul which side of your table is your tool setter usually setup on.
We mounted ours to the very far left it gives enough room for a 15" chuck
and 2 6" double lock vise

Yes.. I moved mine all the way to the left as well because I had a rotary table that fits on the right side.. Seems to work ok (with the IR transceiver) on that side as well..


cheers,
Paul

[Vern Smith]

mgb1974,

In my experience, all the Z offset numbers will be positive numbers in the tool offset table. This does not present a problem as long as you use the probe to set the Z offset for whatever gxxx your program has designated.

It looks strange, but the Z offset numbers in the XYZ offset page (Haas) will be negative while all the tool offset numbers will be positive. I don't like this because I'm not smart enough to figure out how to reconcile them but I would love it if someone would explain it to me.

Vern

[Matt@RFR]

...figure out how to reconcile them but I would love it if someone would explain it to me.

Vern

You mean which way to adjust the H offsets to adjust part thickness? Think of it just like adjusting the tool diameter: Add to the number and take less material. Subtract from the number and you take more material.

The H offsets are, as you know, measuring the distance from the gauge line to the tip of the tool, so if you add, say, .010" to the H offset, the software will raise the head by .010" to comp for a longer tool.

Can you dig it?

[pmurdock]

mgb1974,

In my experience, all the Z offset numbers will be positive numbers in the tool offset table. This does not present a problem as long as you use the probe to set the Z offset for whatever gxxx your program has designated.

It looks strange, but the Z offset numbers in the XYZ offset page (Haas) will be negative while all the tool offset numbers will be positive. I don't like this because I'm not smart enough to figure out how to reconcile them but I would love it if someone would explain it to me.

Vern

If you put your master tool in the spindle and touch off the tool pre-setter the offset should be set to zero. So all the tools are really calculated in reference to your master tool. Say a drill shows an offset of 1.2", which means that its longer by 1.2" than your master tool.

hope that helps!

cheers,
Paul

[Vern Smith]

I wasn't having any problems with the adjustments and their direction, it was trying to figure out where the spindle would end up when I typed G00 Z0 in the MDI screen. I learned my CAM program before my Haas arrived and have used it for almost everything.

Today I took the time to follow all the Z movements through the position screens and finally found my problem. I figured out how to run the table around with MDI entries in X and Y but when I put in G00 Z0 the spindle would head for the table with what appeared to be no intention of ever stopping. Today I figured out this command will run the tool gage line to whatever offset is active unless you input a tool number and tool offset number as well.

Things became a lot clearer from there on.

I'm still a little confused about the master tool. It looks to me like all my tool offsets are the distance from the end of the tool to the gage line. I must have screwed something up in the calibration sequence because there is no way I could have used the gage line for a master tool. Everything works fine however.

I appreciate the help.

Thanks, Vern

[Matt@RFR]

In essence, the PROBE is the master tool, although it doesn't work like paul described. Atleast not with my setup.

If you probe 5 tools, you'll have 5 H offsets all relative to the gauge line. That's it. No master tool involved, and no tools are relative to another.

If I changed any of my tools to be relative to another tool, it'd be all messed up. For instance if I used Paul's

Say a drill shows an offset of 1.2", which means that its longer by 1.2" than your master tool.

, then the control would think I have a drill that is 1.2" down from the gauge line, and that aint right.

And Vern, I always type in my work offset, as well as G80 and G90 when MDI'ing a Z move. There's no such thing as too much information. 'Course that 5% button is my default when in MDI.

[Vern Smith]

Matt,

It sounds like you are getting the same kind of numbers I am and that's good news for me.

As previously states, I have run my machine almost exclusively with my OneCNC CAM software. I even drill holes with it. The arrival of the Renishaw package a couple of months ago forced me to become familiar with the Haas control. I'm about ten percent there. Cloning your lathe tool block has also forced me to learn more than I intended.

I have also found the 5% rapid key to be essential in all situations when I'm doing the programming rather then the CAM software!

Vern

[rbest27]

I had a few issues with mine early on. The batteries went dead pretty quick after I got it up and running. I had my local HFO out and they ran through the whole process with me. Every tech that came out, preferred using VQC to calibrate and use any of the probing. Definately get your software updated if you haven't already. WIPS is crap. VQC is much more user friendly.

[mgb1974]

thanks guys!

I am not sure why Haas even puts in the WIPS program into the control, almost useless.

[Vern Smith]

Here's a little depressing news. My HFO rep. told me Haas is dropping VQC in favor of intuitive programming, how's that for a kick in the a##?

I'm not surprised because I think Haas realizes that many more CAM programs and CAM updates are sold each year than machines, not to mention annual CAM maintenance fees.

With every Haas machine comes a computer and software to operate the machine. It's not a great leap of intuition to envision a Haas CAM program embedded in the Haas control. When you think about it Intuitive programming and VQC are bare bone basic CAM programs.

The next logical step for Haas is a more robust CAM package integrated into the control programming. Their biggest stumbling block will be their crazy typewriter key board and the lack of a mouse. However, lots of folks seem to do well on the lap top computer touch pads.

I wonder if Haas will resist the temptation to make their forthcoming CAM package an extra cost option. A real 3D simulation display may even be included, how nice would that be, that alone would sell a bunch of them.

Vern

[Stabbinhobomill]

I have the renishaw Touch off tool probe,and the program zero probe that is in the tool holder with the rest of my tools..For most parts i like my Z0 to be the highest surface i will actually be machining on.
I just touch all of my tools i will be machining with by hitting Edit,then F1(i think,my fingers do the thinking for me there lol) go into then the visual quick code and go to the tool one,and go to random tool,so i can touch off 20 or so tools.and then to touch off for program zero. and go into my probe programs there(edit,F1,then go into the probe and tell it Probe z surface, or an x or y web,or pocket or just pos.,or neg., surface touch offs.got to be within .400 approx. from your surface you will be touching.i just eyeball it.
and then Im ready to program. ex.
T3M06
M03S2800
G00G90G54X1.Y0.
G00G43H3Z1.
now ready to hog some metal off..



about your probe open alarm, as far as i can remember from my experiences with them 3 things cause this.
1.Batterys are dead
2.inside of probe head is unclean,i just moved the stylus around with my fingers in all direction for a while to free up the tip,coolant or something got into it
3. The probe cannot communicate with the reader(mounted to your machine wall)
and for safety will not move.if the probe continues with its program,and it cannot transmit a signal to the reader it will just keep going its programmed number until it crashes.because it cannot tell the machine to stop.

Its a bummer sometimes to use the probe down inside a part.as the probe cannot communicate when something is blocking its view to the reader .