Haas tool offsets and work setting - is there a better way

Hi All

Just had my Mini Mill delivered and took the days training with the Haas engineer. When it came time to look at tool offsets and work off sets I was left scratching my head somewhat. Granted this is a move up from a home built hobby machine running linuxCNC but the way they showed me to do it seemed convoluted and strange.

As I'm sure you all know I was shown to set all tools at a certain height. Let's call that height 'A' and 'A' is now a datum as such. That's set all the tool compensation lengths.
Moving to the work offsets X and Y seem to be normal but coming to the 'Z' I had to measure this as the difference between the above datum 'A' and the work top and offset it manually.

Now the problems with this is as follows:
When I set the datum: to remember it I would have to zero the operator read out - this however isn't remembered by the machine after a power down so in a morning I would have to measure a tool/haimer off this datum to then get the value again to be able to crack on. Seems strange to me. Having to do this all manually seems time consuming too.
The readout also didn't change as far as I could see but maybe this was to do with the coordinate system I used, maybe I hope that anyway. With linuxCNC I would touch off, set zero then the display read zero. MDI commands were then very easy....

Question:
Is there a way to do it where I measure a 'reference' tool (say the haimer) and then measure the difference between the length of the Haimer and the other tools I am using. Those values being stored as a positive or negative difference. Then I could just zero the Haimer from the top of the work piece when needed and all is done.

Next question:
What's the process you all use to set your heights. If there is no easier way than this are there any tricks to make it quicker.

Thanks

Jools

That's why we opted for the probing system when we ordered our VF2YT. Unfortunately I don't a good answer for your direct question.

Where to start.... First, may want to do some reading here, lots and lots of info on tool and work offset setting.... If I didn't have a probe, I would touch all tools on a 1x2x3 block (any side, as long as it's parallel), then using an indicator and the operator position readout, <position> , arrow over to operator, select hand jog then z axis, with your indicator reading zero on your 1x2x3 block, hit origin, dial indicator to zero on your workpeice, enter this number + or - on your G54 Z work offset page.

edit: assuming NGC

JustAbout said:

That's why we opted for the probing system when we ordered our VF2YT. Unfortunately I don't a good answer for your direct question.

Click to expand...

I would love that. Can't afford it right now though

Mike1974 said:

Where to start.... First, may want to do some reading here, lots and lots of info on tool and work offset setting.... If I didn't have a probe, I would touch all tools on a 1x2x3 block (any side, as long as it's parallel), then using an indicator and the operator position readout, <position> , arrow over to operator, select hand jog then z axis, with your indicator reading zero on your 1x2x3 block, hit origin, dial indicator to zero on your workpeice, enter this number + or - on your G54 Z work offset page.

edit: assuming NGC

Click to expand...

Yeah that's the way I was shown and understand it to be. Just seems convoluted and wondered if there was an easier/simpler way

Book way is the "safe" way as it minimises the risk of an "oh sh*t" moment when what you have stored as areference isn't what you think you have stored.

Awfully easy with CNC to do shortcut procedures that work just fine on the job I'm doing right now but leave you ass hanging naked in the wind should you get problems with a different job.

In an industrial situation everyone working a standard way is the only way to keep proper tabs on WTHIGO. Initially it might not seem so important for one guy in his own shop but eventually you will do enough jobs that figuring out the easy way for each one no longer hacks it.

Clive

In a nutshell, the control adds the G54 Z value to the tool offset length and that's how far in Z the machine travels to get to the workpiece.

There's basically 3 common ways to set your Z's.
1) Set G54 Z to zero.
Touch all your tools off the top of the work.
Done. Sometimes called "air gap" method.

The downside to this is if you are using multiple work coords you will need to touch each tool off each workface needing multiple TLO's for each tool. You will also need to turn off the "H&T agreement" setting which some people don't like to do.

2) The way you currently do it. Touch tools off a "datum".
Measure from datum to work face and put this value in for G54 Z. If your work is higher than your "datum" the value will be +. Lower, -.


3) Touch the spindle face off your datum. Enter this as G54 Z. (It's going to be a big -Z.)
Active G54 in MDI.
Touch tools off datum. All tools will now have a + TLO. (It is actually the length from the face of the spindle to the tip of the tool)
Touch your spindle off each workpiece face and put this into each work coord you're using.

Probing systems and offline tool presetters use this method. Sometimes called "gage length" method.

This is what I used to do on my machine without probing:
Buy one of the tool setting blocks that lights up when you touch off a tool. We had a Fowler.
Use the block in only one spot on the table for consistency. We used the flat behind the dead side jaw on the Kurt that was normally on that machine.
Touch off all the tools to that block including the Haimer. All tools are now set relative to each other and the Haimer.
We left the Haimer set up as tool 20 in that machine unless that spot was needed in the program.
Put the work piece in and find edges with Haimer as normal using the part zero set button to set the work offset.
Add the length of the Haimer to whatever value was written for z in the work offset(when you hit part zero set button).
All tools are now set relative to the top of the part.
By leaving the Haimer set up as one tool it is easy to toggle from the work offset screen to the tool offset screen to verify the value for the Haimer.
You could write that value on a sticky note and stick it on the control somewhere or write it to an unused tool offset as you have more tool offsets available than spots in the changer.
I think the display defaults to G54, but as soon as the control reads a different work offset it will change to G55, G56, Etc.
You can press the position button to scroll to the work offset display.

jools said:

Yeah that's the way I was shown and understand it to be. Just seems convoluted and wondered if there was an easier/simpler way

Click to expand...

Kind of standard IMO, but there are a few ways to do it. This seems pretty straight forward to me. You have to touch your tools somewhere (unless you have a pre-setter, but a decent one is half as much as a probe package so..). Your Z offset and tool offsets should not change, unless you change them. With the method I presented, if you have some common tools, you don't have to re-touch them, just need to re-touch your part and change your G54 Z offset.

Thanks for the responses guys and or gals

Looks like I just have to learn a new way. Once I've done it a few times I'm sure it will become natural to me

Thanks for the help

If you want to do the easiest way, until you decide which way you want to do it in the future, is simply to touch each tool off of the top of your part and set that as your tool zero length.

Just make the top of the part the zero for the part and touch off each tool. Works every time.

I just touch off each tool by rolling a 1/2" pin between the tool and part then hit tool set. G54 Z has -0.500. Rather difficult to touch off a tool directly to the part without mashing into it.

magno_grail said:

I just touch off each tool by rolling a 1/2" pin between the tool and part then hit tool set. G54 Z has -0.500. Rather difficult to touch off a tool directly to the part without mashing into it.

Click to expand...

I just slide a piece of paper under it until it hits or drags. Then depending on hit or drag it goes down another .003" or .004". Works every time. I also use a 4.0" touch off gauge then add the 4". Easy peasy.

From your description, it sounds like you are using the same procedure I am using or something very close to it. This is the process we use at our shop:

Installing a new tool:
1) New tool is placed in spindle
2) An Edge tool height gage is placed on the table
3) The tool is lowered to the gage then the Tool Offset Measure button is pressed which sets the Tool height to 4" above the table

The daily startup routine:
1) When the machine is first turned on, the Haimer 3d sensor is placed in the spindle
2) Two 1-2-3 block are stacked on the table to give a 4" height
3) The Haimer is lowered to the top of the 1-2-3 blocks to its zero point
4) Go to the Operator position screen and press Z followed by Origin to zero the Operator Z Position

Loading a work piece:
1) Work piece is loaded
2) The Haimer is placed in the spindle, then lowered to the Z origin of the part
3) On the Offset screen, the cursor is moved to the G54 Z field
4) The value displayed in the Operator Z position is manually typed in followed by pressing F1
This process basically lets the machine do the calculation for you from the tool offset (4" from table) to the part Z origin.

As you mentioned, the operator Z resets after the power is cycled. Initially I thought this added work to re-set the Operator Z position every time the machine was turned on. I eventually convinced myself this was a good thing because when the machine homes, it may vary a little from one startup to another, so re-setting the Z ensures a more accurate position.

What exactly are some of you blokes going on about daily startup routine, machine resets this or forgets that upon power-up?

The control doesn't forget a f@cking thing, nor do you have to do diddly in the morning!

Read the manual and figure out how Setting 64 - "T. OFS Meas Uses Work" functions!

I know, Ex-factory Setting 64 is always set to be ON because Haas cannot figure out how to properly incorporate a fucking probe for workoffset pickups on their machines,
but for folks who do not have a probe or toolsetter, Setting 64 should be OFF so you can pick up your tools independent of the active workoffset.

Worse yet, the Haas "guru" with his "Tips and Tricks" video on workoffset pickup is EXACTLY why we're still discussing tool and work offset pickup methods in 2020!

SeymourDumore said:

What exactly are some of you blokes going on about daily startup routine, machine resets this or forgets that upon power-up?

Click to expand...

Yeah I'm confused by this too. On our Haas machines that don't have probing, I pick up all the tools off a height setter which I put on the table. Similar to this one:
Touch Off Gage

After I've picked up the last tool, instead of hitting "Next Tool" I hit MDI then hit JOG again which only serves the purpose of conveniently zeroing out one of the "digital readout" displays (I think it's Distance To Go), then with that same tool I jog over and touch off what I want to be Z Zero on the part and put that Z number from the readout into the fixture offset Z register. I hope that's clear, it's really simple. Seems like I typed a lot to explain it.

One advantage to this is that all your tools are picked up off a central location and it's your fixture offsets that vary in Z. This is good because if you need to sneak in a quick job on the side and you want to use some of the tools you have in there already, they are already picked up.

Volitan said:

After I've picked up the last tool, instead of hitting "Next Tool" I hit MDI then hit JOG again which only serves the purpose of conveniently zeroing out one of the "digital readout" displays (I think it's Distance To Go), then with that same tool I jog over and touch off what I want to be Z Zero on the part and put that Z number from the readout into the fixture offset Z register. I hope that's clear, it's really simple.

Click to expand...

Does your Distance to Go or whatever setting you say zero's out, hold that value all the time including after a power cycle? I use the User Position Z coordinate as my reference for tool offset which is the value that resets through a power cycle.

arj3090 said:

Does your Distance to Go or whatever setting you say zero's out, hold that value all the time including after a power cycle? I use the User Position Z coordinate as my reference for tool offset which is the value that resets through a power cycle.

Click to expand...

No it gets zeroed out all the time. I just read your procedure and it looks like we're doing the same thing as far as zeroing out where the tools were picked up from and going to the part and putting the value in the fixture offset Z. I don't do it everyday though, just once when I pick up the job. I trust the machine to be in the same spot when it homes in the morning. It's not like it hits a switch and calls that home, it goes until it hits a switch (or sensor) then backs up until it sees the Z channel on the encoder and calls that home. This way the screw is in the exact same spot every morning.

Those Haimers are nice, my buddy has one.

All the machine wants to know is the height of your tools to the work piece. A nice shortcut is to just measure your tools to a point on the table make sure those go into your tool length offsets and then use a fixture offset for your part top and that distance is measured from the point that you used to measure your tools to the top of your part. Maybe I didnt read all the replies but doing it this way helps you from having to touch off each tool on the top of the part