Setting reference tool for G7 Rotated planes on DMU50V

I accidentally changed the reference tool data for my DMU50v with Millplus 4.0 control. Its somehow supposed to reference the tip of your tools to the face of the spindle in relation to the table surface. If not done correctly, when the machine rotates to tilted planes, the zero point shifts to the wrong place.

I had a guy at DMG walk me through the procedure a few years ago, but didnt write it down. Called DMG this AM but the guy who I was referred to today didnt know either. Its not in any of manuals I have, or in the G7 setup documents. Maybe considered a service thing?

Anyone know the procedure? I kinda needed to make some parts today. Tried a few times to set it the way it made sense but my zero point is now 4=5" off when axis are rotated!

Ok so there's no one whos using a DMG machine with millplus control and no one whos ever referenced a tool tip to the spindle face to allow your tool to remain aligned to the reference zero when rotating the planes in G7? How do you guys ever get any parts made??

We have sorted this out.

If anyone has questions about this they can contact me.

Regards,

Dave @ Nerv Industries Ltd

Yes indeed, Thanks Dave!!

Well, forum etiquette is that you post the fix here, so that 6 years from now, when someone google searches the same or similar problem, and stumbles across this thread, they don't just see "I fixed the problem", they get an answer so they can fix their own problem.

"Contact me"... What if you drop off the forum for whatever reason? What if you change emails? What if you have a stroke tomorrow?

Not saying you have to share if you think you have some proprietary fix or anything... But it's the nice way to do things.

TeachMePlease said:

Well, forum etiquette is that you post the fix here, so that 6 years from now, when someone google searches the same or similar problem, and stumbles across this thread, they don't just see "I fixed the problem", they get an answer so they can fix their own problem.

"Contact me"... What if you drop off the forum for whatever reason? What if you change emails? What if you have a stroke tomorrow?

Not saying you have to share if you think you have some proprietary fix or anything... But it's the nice way to do things.

Click to expand...

Yeah teach I agree!

It ain't cool to show up here ask a question then get the matter sorted offline without returning with the solution.

Thanks to Dave but it is best to have the solution right here on the board to stay for years to come. It's how this whole thing works.

Brent

Sorry for the delay, busy monday.

Ok, here it is Dave please correct me if Im wrong anywhere along the line.


First, remove the tool from the pocket that you will be using for a reference tool.

(I keep a 3d taster in that tool pocket for setting comparative Z height of tools and the Z height of parts)




Go to CONTROL go to TOOL offsets

The tool in the spindle will be at the top of the tool table and will be highlighted
Set L1 in that tool to "0"

Go to MDI Enter G53 press enter

Setup a 7" tall stack of 123 blocks. (has to be at least 7" as the spindle face wont get closer to the table than that)

Be sure to measure the blocks with a Mic as even a small deviation will throw off the alignment



Go to MANUAL in control, make G54 I2 active. (make sure that there is no offset active in G54 I2 if so zero it)


Move spindle face to touch the 7" stack. (Heres Daves suggestion on that)

take a 1" round, bring spindle face slightly closer than the distance, roll the round under the spindle until it just clears

Enter 7" into the Z height in the G54 I2 offset

Put your reference tool back into the same tool pocket and load it.

Bring the tool to touch the 7" stack


Go to MANUAL, FST, enter "0" into the Z line, press the Z tool offset button

In L1 you will see a positive number.

Now anytime you need to set tools, you set your Z using the reference tool at "0", using the same 7" block, then touch off all your tools to match that "0" point. (I use a 4" toolsetter atop a 3" 123 block for this)

No matter what G54 you are in, its still referenced to the face of the spindle.


This is the only 5 axis machine Ive ever touched so Im not sure how its implemented on other machines. This procedure is not in any of the manuals I have or in the G7 setup pages from DMG.

I think Dave just figured it out. Personally Im barely smart enough to run this thing, once I get an operation running Ok, I dont revisit it again unless it breaks.

Id be curious to hear how its done in other 5 ax machines.