[BBQ70]

I am machining on a VF5 with 4th axis. I have to rotate the 4th axis to load each part on the fixture. Unfortunatly in hand jog mode it highlights the "H" lenght for the tool in the spindle. When I pushed the "Chip FWD" button to remove some chips while I loaded parts I must have Hit the "Tool Offset Measure" button by mistake since it is right above the Chip FWD button. This unfortunatly cleared the tool lenght without me realizing it. As you can guess as soon as I hit cycle start I buried the tool into the fixture. So does anyone have any suggestions as how to safeguard from having this happen again.

[Geof]

This puzzles me. If the tool offset is zero the tool is going to stay at the tool change height. Unless of course you have a large negative Z in the work zero so you are working your tool offsets from the table or 4th axis centerline.

How do you normally set up your tool offsets?

[BBQ70]

I use a Renishaw Probe to set the tools and work offset. This gives me a positive number for my tool lenght and the work offset is a negative number. My g54 Z 0. is the center of the 4th axis. My original T6 lenght was around 6.1 and since the machine was at tool change position (Z 0.) when I must have hit the tool offset button I lost my tool lenght.

[Geof]

I use a Renishaw Probe to set the tools and work offset. This gives me a positive number for my tool lenght and the work offset is a negative number....

I do not use probes and this is one of the reasons; I do not like positive numbers for the tool offset and I never use them.

When you have a positive number and accidentally erase it the tool goes too far down; with a negative number the tool stays too high, I prefer too high.

I have no idea how you can guard against it happening in the future as long as you use positive tool offsets.

[Delw]

WOw I never thought of this, until you 2 pointed it out, about the positive offsets, That is pretty dangerous.
POS numbers are never good on machine offsets.

On my machine theres a permission that if I apply number that is xx amount the machine will ask me if I am sure I want to add it, gives me a yes or no screen. it works on the fixture offsets , is your permission enabled for that? would that prevent something like this happening?
its annoying but a few times I have missed a decimal cause I font have my glass's on or typing to fast and it saved my butt.

Delw

[BBQ70]

If I type in a number it asks if I am sure and I have to hit Y to verify, but when I hit the tool offset it does not ask if I am sure. Is there a setting that I can turn on for the Tool Offset Measure to ask if I am sure because that would have prevented this from happening.

As far as using the probe for setting the tools this is all I have used. I will have to spend some time and learn to set tools with out the probe. Since I have only used the probe I have never used the tool offset button so I never thought about accidentally hitting it and what problems it could create.

[Delw]

I never use the tool offset button either, only the probe. I just assumed.
when I first got the machine I hit it by accident , we were using one tool to test the new spindle on some cuts(tool 1). The tech was there, I said **** that button isnt safe, he told me not to worry about it, it didnt change your setting. I said ok and left it at that.
It could have been that I wasnt in the correct mode/screen?
when I see him or talk to them again I will ask them about it, cause now I am curious.

[steedspeed]

I set my face mill as zero then make all the other tools relative to that. Some are + and some are -. Works like setting lathe tools so then you just face a piece and press the set workpiece z zero to set work Z offset.

[mactec54]

Hi BBQ70

You can not do what you said happened you can not change the tool offset unless the tool offset page is open

You can press the button Toolset all day & it will not change any offsets something else
happened but it was not because you pressed the wrong button

Just remember the Tool Off Set Page Has To Be Open For this to happen

It is a rear thing that you need to have any tool set Positive No Tools should ever have to be a positive number this is a crash waiting to happen

[BBQ70]

mactec54,

When I push the hand jog button the tool offset screen in the top right turns white and the memory screen on the left side turns blue with the machine offset screen lower right stays blue. It also highlight the tool that is in the spindle, which for me is t6. Every time I then push the Tool Offset button it changes the tool lenght to 0. since I am at tool change position ( home ). I have repeated this several times to verify what had happened and it always does the same thing.

[HuFlungDung]

I'm pretty much with Geof for the same reasons.....old school reasons, but there were reasons for the reasons

Is setting 64 the one you have to change "tool offset measure uses work" if you want to use negative offsets? I don't use a probe and mine is "off".

However, I think if you have 64 "Off", then Offset measure does not perform a useful function in setting a Z0 in the workshift, but its still useful for X and Y. At least as far as I know, I have to measure the distance from the tool setting plane and the Z0 of the part, and type in the Z value per each workshift.

I don't see why you could not use a probe and also have 64 off. It should then ignore the distance between the gauge plane of the spindle and the tool, which is why it is giving you positive tool lengths. But I'm asking this, not suggesting it, because I've not played around with it.

[fuzzyracing1967]

Short of changing the way you get your offsets by probing ,( I say if your familar with doing something one way keep doing it that way).The only thing I can think of whould be to turn on setting 119, it is a offset lock.Sure beats crashing

[Geof]

mactec54,

When I push the hand jog button the tool offset screen in the top right turns white and the memory screen on the left side turns blue with the machine offset screen lower right stays blue. It also highlight the tool that is in the spindle, which for me is t6. Every time I then push the Tool Offset button it changes the tool lenght to 0. since I am at tool change position ( home ). I have repeated this several times to verify what had happened and it always does the same thing.

From your description you have the latest control; what mactec54 says is correct for the older controls.

I would contact Haas directly and complain that this is a glitch that should not be there; or maybe Haas Apps will see this thread and comment.


Setting 64 simply subtracts any Z value in the work coordinate page from the tool length distance; I think it will not affect what happened.

[gpcoe]

I've been bit by the positive T offset bug and yes it's a crash waiting to happen. My idea though I haven't implemented it yet, would be to write a variable alarm that checks the height offset page before running the g43 line. The shortest tool holders we have are maybe 2.5 inches or so and I'd set it to alarm if there's a number less than that in the offset page or something. #3026 is the tool number currently in the spindle and (though I don't have them in front of me) I beleive the H offset variables have a number corresponding to the tool #. IE #5021 would be H offset for T21. So it might look like this:

T21 M6
IF [#[5000+#3026] LT 2.5] THEN #3000= 1 (HEIGHT OFFSET UNDERSIZED)
...your program

We use positive offsets because we have a parlec height setter for the shop. If I were to strike and not use this method I'd probably be in trouble when a 2nd shifter does it the "normal way" or something, so I'm stuck with it.

Anyway, just a thought. You'd have to have macro variables unlocked to use this type method obviously.

Greg

[mactec54]

HI BBQ70

How old is your machine & what is your software version

Once you have done your tool offsets that window/page should be closed then it is not active & this can not happen

It seems you are leaving the offset page open this is not a good thing to do this must be closed when you have finished setting your tools

[BBQ70]

Mactec54,

The machine is 10 month old, but I have no idea how to tell what version I have. I will try to find out and let you know. I do know it is the new control.

As far as leaving the offset page open, I am not sure how to close it. It seems like it defaults to the tool offset window every time I hit Hand Jog. Even if in Hand Jog mode I make the work offset page active , then go to Mem and back to Hand Jog, it is back to the Tool Offset window.

[Delw]

I will check mine later today.
I tired it yesterday a little bit with hitting the jog key and did not get the same result.

Maybe if while your in jog and you hit page up or down or settings you will get a different page, then when you hit mem or another button it saves the last page in the jog mode. so when you go back to jog that offset page wont be there your last page in the jog mode will be? I am sure we have the same software as our machines are pretty close to the same date.

[BBQ70]

I'm begining to see that there are some down sides to making these machines so simple to run. You buy a machine and they spend 4 - 6 hrs with you and within a couple of days you are running parts for the first time. The problem is for example with the probe, you put a tool in the machine hit a button and the machine does the rest. Without understanding how or why, your tool is now set. This ease of running the machine is taking the thinking out of it. I am now seeing the importants of learning what is happening shall we say behind the scenes.

[Delw]

BBQ70
your 100% correct the new machines do that. I just checked mine (vf2 ss new) and did exactly what yours did. scarey ****.

so heres a way around it.
once you power up hit job, you will be on the offset page like you describe. page down to the offsets are like on 100 something, or something you dont use.

then you should be safe for the rest of the day. as when you hit jog anytime during the day (as long as you dont power off) it will come up to that last offset.

Now the only thing I didnt check was to see if it worked when you change tools, ie if the page will stay at the same number or automatically goto that new tool called out.
I got a stainless job running in it other wise I would play with it some more.

if it reverts back to the number of the tool currently in the changer after a tool change is called there might be a parameter or setting that could be changed for the default?

Glad you brought this up, cause I got fat fingers as well.

Thansk Man
Delw

[BBQ70]

If i scroll down to another tool say 100 it will stay there untill it makes a tool change, then it goes back to what is in the spindle. I am going to call HAAS and see if there is a parameter that can be set or changed to prevent this again.