What's new
What's new

Z height issues

Kfstudios

Plastic
Joined
Feb 6, 2023
First post to practical machinist very new to the forum but looking for any help possible with this issue I am having. Here’s the run down I’ve been having a bunch of issues with z heights on my haas vf3 I believe it’s a 94. I am currently facing a plate from .167” to .161” final thickness. I touch my insert mill off to the bottom of my part and have a z positive in my program to z.161 after the program cycle I’m getting .156” thickness on the part. I have run thru the z backlash test with about .0003” difference. I have also verified all 4 inserts on the insert mill are within a few tenths of each other. Any input would be greatly appreciated.
 
How exactly are you performing this step?


Does this repeat from part to part?
I am touching off to a .5000” gauge block on the surface I am setting the parts on then adding a -.5000” to my height offset. So far every part is doing the same thing.
 
Is this thickness after machining consistent over the entire surface of the part, or possibly thinner in the middle than around the edges? What material. How big? How is it being held? How big of facemill?

If you're using high positive rake inserts, they will want to suck the part right off the table, and will generally over-cut anything that isn't held down firmly. If the plate is aluminum at the thickness mentioned, and it is only clamped around the edges, I can see an excess five thou coming off no problem if the cut is even sort of aggressive.

EDIT IT: You getting any chatter?
 
Last edited:
Is this thickness after machining consistent over the entire surface of the part, or possibly thinner in the middle than around the edges? What material. How big? How is it being held? How big of facemill?

If you're using high positive rake inserts, they will want to suck the part right off the table, and will generally over-cut anything that isn't held down firmly. If the plate is aluminum at the thickness mentioned, and it is only clamped around the edges, I can see an excess five thou coming off no problem if the cut is even sort of aggressive.

EDIT IT: You getting any chatter?
The material is D2 2” wide i am holding the material in a vice sitting on a shelf about .250” wide so about 1.5” of the part is floating but the part is coming in at the same thickness even where it’s sitting flat on the shelf. I am running a 1” 4 flute insert mill.
 

Attachments

  • D6FA3CD7-955D-48DD-8102-65CD723F81FA.jpeg
    D6FA3CD7-955D-48DD-8102-65CD723F81FA.jpeg
    1.4 MB · Views: 40
Maybe widen that shot so we can see the entire setup.

I'd re-do your tool height measurements just to be sure. If they come out the same, then the problem has got to be looseness in the machine spindle or axis screw or setup. Especially 5 thou worth.

You could try Single Direction Positioning, by bring your tool down at a rapid rate say 50 thou below the cut height, then feed it back up to your cutting Z height.

The rapid move below the part will throw any looseness in the Z axis against the top of the ballnut and essentially load the screw like you would on a manual mill, where you turn past your mark and come back. Anyway... if this changes the situation it pretty much says machine wear in the Z axis. (Spindle bearings or screw/nut.)

One last thing. Check your micrometer against that 0.5000 gauge block and make sure it's reading right.
 
Maybe widen that shot so we can see the entire setup.

I'd re-do your tool height measurements just to be sure. If they come out the same, then the problem has got to be looseness in the machine spindle or axis screw or setup. Especially 5 thou worth.

You could try Single Direction Positioning, by bring your tool down at a rapid rate say 50 thou below the cut height, then feed it back up to your cutting Z height.

The rapid move below the part will throw any looseness in the Z axis against the top of the ballnut and essentially load the screw like you would on a manual mill, where you turn past your mark and come back. Anyway... if this changes the situation it pretty much says machine wear in the Z axis. (Spindle bearings or screw/nut.)

One last thing. Check your micrometer against that 0.5000 gauge block and make sure it's reading right.
So I did verify my micrometer to the .5000” gauge block it ready perfect and verified with a 1.000” standard just to make sure everything on the measurement side is good. I am starting to lean more towards spindle issues due to the fact we can’t run over about 3800 rpm without terrible spindle sounds. This machine was very neglected before we got it. I’ll do more of the tests your talking about when I go back to the shop everything you have described makes perfect sense.
 
I am touching off to a .5000” gauge block on the surface I am setting the parts on then adding a -.5000” to my height offset. So far every part is doing the same thing.
Somehow your part is sitting .005" higher than the measured surface. Either the part is lifting in the vise or the corners of the workpiece are interfering with the inside corners of the jaws.
 
Somehow your part is sitting .005" higher than the measured surface. Either the part is lifting in the vise or the corners of the workpiece are interfering with the inside corners of the jaws.
Yes... this sounds like the best and simplest place to start your quest. Wish I'd thought of it myself. If this doesn't pan out, then try looking into some of the other stuff.

Troubles at 3800 rpm? Is this a CNC knee mill of sorts? Head tram-able? I suppose with a 1" cutter it wouldn't matter much anyway if it was slightly out of tram. Nor would the offset measurement change much regardless of what side of the tool it was measured on.
 
Are you checking your entire part for thickness? Is it possible that it's bowing upward when the vice is tightened?

If currently touching off on the top of the material, it's considerably easier (and faster, and possibly more accurate) to use a .5000" dowel pin.
Bring the cutter down to less than .500" above the material, then roll the pin up against the cutting edge and apply just a touch of pressure on the pin against the cutting edge. Bring the spindle *up" until it's close to where the dowel pin would roll under, then switch to.0001" steps and bring it up until the dowel pin rolls under the cutting edge. It's relatively easy to set height within one or two tenths using this method, and far less chance of damaging the cutting edge by bringing it "down" on a gage block. (IMO)

PM
 
Yes... this sounds like the best and simplest place to start your quest. Wish I'd thought of it myself. If this doesn't pan out, then try looking into some of the other stuff.

Troubles at 3800 rpm? Is this a CNC knee mill of sorts? Head tram-able? I suppose with a 1" cutter it wouldn't matter much anyway if it was slightly out of tram. Nor would the offset measurement change much regardless of what side of the tool it was measured on.
The machine we are running is a haas vf3 I believe it’s from 94 so it is older and was very poorly taken care of before we got it.
 
Are you checking your entire part for thickness? Is it possible that it's bowing upward when the vice is tightened?

If currently touching off on the top of the material, it's considerably easier (and faster, and possibly more accurate) to use a .5000" dowel pin.
Bring the cutter down to less than .500" above the material, then roll the pin up against the cutting edge and apply just a touch of pressure on the pin against the cutting edge. Bring the spindle *up" until it's close to where the dowel pin would roll under, then switch to.0001" steps and bring it up until the dowel pin rolls under the cutting edge. It's relatively easy to set height within one or two tenths using this method, and far less chance of damaging the cutting edge by bringing it "down" on a gage block. (IMO)

PM
I’ve checked across the whole part for thickness and it’s holding within about half a thousandths everywhere so I’m not thinking it’s bowing when we’re clamping we have also put a indicator on the part when we clamp and it’s not moving at all. So right now we are touching off on our surface the part is resting on and running that as our z zero then all program z heights are positive I’m touching off using that same method but with a gauge block instead of a dowel but I’m going to try the dowel method also just to see what we get with that.
 
Even when I program the z height on something dead flat like our magnet it always cuts deep. .005 seems like user error. I tend to find when I pick up this way it cuts .0015 -.002 deep.
 
I would look at the numbers as the program runs just to make sure the tool is indeed going to the correct height. My guess however is that the vice is lifting as you tighten it. Put an indicator on your workpiece and have a look as you tighten it.
 
I was just going to say this. How much time and effort are you wasting.
Move up your Z the. 005" and rip yiur parts out.

You admit to having a neglected 28 yr old haas. You say it always cuts .002" deep, then pickup. 002" higher and get to work.
 
Smack that thang wit a dead blow mallet.

It's a strip of metal, it can bow from the clamping pressure. It could also be crusty stuff or burrs on the edges. And if your vise jaw surface isn't perfectly sharp-cornered, the part could be sitting at the top of the tiny fillet. The vise itself can easily have 5 thou jaw lift.
 
Way out there suggestion, is there a negative value in the tool offset wear register or something in the G53 Z (that's Fanuc, not sure what Haas calls the common offset)?
 








 
Back
Top