The Mystery of Z offset

[Swede]

I am going nuts trying to execute Z offset with my bench mill! I waste more time setting up tool changes than anything, it's getting to where I am executing machining operations with a less than perfect tool because it's simply easier.

The spindle is an ER-16 collet nose. I am using Visual Mill and Flashcut. The end mills are normal single-end cutters.

How do you guys set up Z for precision metal work? I really don't want to modify the spindle (yet) for QC tools. Hints and tricks are greatly appreciated!

[cbcnc]

Hi Swede,

There is a thread on just that on the Cad_Cam @Yahoo group.
Cad_Cam_Edm_Dro
The consensus of it is that you set your Z as close as posible by eye or touch on a piece of scrap. Then you take a test cut and measure the depth. Then go back and readjust your settings.
I understand your frustration as the setup time far outweighs the actual machining time.
Good luck!
By the way, you have a very interesting website.

Chris

[Ken_Shea]

Hi Swede,
Ah yes, tool offsets, work offsets, Z offsets, tool compensation, just a bit confusing is it?
I am just getting the hang of it my self Swede and totally unfamiliar with your controller, but.....
All CNC machines must have some type of tool register built into the controller software where you input the tool height and diameter of each end cutter, drill etc. that you will use in a given program. This tool height measurement needs to be from a consistent point on all tools all the time. (The table normally) I use a 1-2-3 Block on the 2" side always. Once you get the tool height set on and entered your CNC machine needs to know where the top of your part is, this is where you have to look at your setup to see how this is entered. On my controller once I have the tool height set in the Tool registry I zero the z value while the tool is on the 2" block (actually I stop going down when the paper drags, remove the block and go down another .003), then jog over and down to top of part, take the Z position and use that Z position for the Z value in G54 or whatever work offset you are using. You will also need to jog over to whatever position represents x and Y zero on the fixtured part and enter those positions into G54 X and Y work offsets.



A collet will make this a little more problematic since you cannot set each tool and install them as needed as you could with say a CAT30/40/50 type holder.

Hope this makes some sense and not further confuse


Ken

Here is a link I really like
http://www.mmsonline.com/articles/cnc9801.html

[duluthboat]

If you want to find the height of any tool above the stock a quick, easy, and accurate way is to use a pin of known diameter, like a dowel pin. Run the Z down (spindle OFF) over the stock so that it is lower than the diameter of the pin than slowly raise the Z until the pin just rolls under cutter. You now know the exact height of the tool off the stock. How you enter this value is different on most controllers.

Gary

[SJ781]

If you are talking about the tool repeating in the collet..... Build a stop that the base of all the tools can but up against in the collet holder. A lot of cnc tool holders have a set screw in the center of the holder so you can adjust for the base of the tool to hit against. It needs to be attached inside the collet holder or spindle not the collets because the height can change alot with a slight bit if change in diameter on the tools. If the stop is in the spindle or collet holder the action of the collet as it's being tightened will draw the tool tight against the stop. Then you can change tools and collets and still have a reference point in the collet holder or spindle. Maybe this is clear enough, can't think of a better way to describe it...

[Mortek]

I use the handwheel (you have to have one though) and bring the tool down to where I can still see some light between the tool and the workpiece. Then I get a piece of .001 shim stock and jog down .001 at a time till the shimstock won't slide out. Then I take the shim out and go down .001 to account for the shim and set the z. This works great for me and I find if I am using up to 12 tool that all cuts blend very well.

[lsfoils]

this should proly work. My boss' machine is set up to find the surface and account for tool length using balsaman's method. Not sure which controller you'd have to use.

http://www.cnczone.com/forums/showth...&threadid=3836

Gonna be finding out soon, myself.

[Swede]

Thanks for all the great suggestions! My problem was really evident when I was trying a 3d mill job. I initially used the stock for Z=0. Of course, the stock was soon gone, and setting the ball mill to Z=0 was tricky. I think ultimately I'd like to find a miniature QC system.

I did find a simple answer for 1/8" bits in a collet system. You can buy the little plastic collars which are often found on 1/8" carbide drills from Drill Bit City

http://www.store.yahoo.com/drillcity/toolac.html

I made an overbuilt ring setter out of an old slide, collet holder, and a .0001" plunge indicator. Maybe this will help someone else, at least for 1/8" bits. It would be nice to find rings like these for 3/16" and 1/4" shanked tools.

[RotarySMP]

I took some time in the machine shop of Dallas Airmotive last time we had an engine in. One of the machinists was just zeroing a whole set of tools in their QC holders before running a program. He used a small, expensive looking device about 3/4" round and 1" high which obviously had a very sensitive and repeatable contact in it, which made a ring of LED's around the periphery light when touched.

Put the device on the bed or fixture,then just touched off each tool multiple times switching to a finer jog increment each time.

[Al_The_Man]

If that was a Renishaw, depending on the model cost from $9k to $15k. I have used one (not mine) that fits in the spindle and is cordless (infrared) and you spin the spindle cw to turn on ccw to turn off.
Neat but expensive.
Al

[HomeCNC]

Swede,

This is exactly why I built my fixed tooling for my Porter cable router. http://cnczone.com/forums/showthread...2&pagenumber=6

Look at post #70. I now use G54 for offseting my work from my home position and telling where my Z height is, and I use G43 for using tool lenght offsets. This setup works great! I have been thinking of doing a white paper on this setup for the Zone, just don't seem to find the time.