Probing datums as called out on the print

[cgrim3]

I have a question for the machining community. A lot of my work involves making parts from drawings with a lot of GD&T called out.

Say I have a raw block that I want to machine (contour the outside and drill a hole in the middle). I set my G54 as the corner of the stock. I contour machine the outside of the block and facemill the top. Most endmills are ground .001" undersize so without adjusting any of my wear offsets for the endmill, the block will be .001" - .002" oversize in both directions when mic'd.

Note that datum A is the top of my block (after facemilling), datum B is one of the sides (after contouring), and datum C is another side (after contouring).

Now, I want to drill a hole in the center of my block. The hole has a true position tolerance of .001 relative to datums A, B, and C. True position of .001 is equivalent to +-.00035". My block is slightly larger in both directions from contouring with a slightly undersized endmill, so if I drill my hole in the center of my block, the hole will be out of tolerance.

Possibly the only way to hold a .001 true position tolerance on the hole is to reestablish your G54 by probing datum B and datum C after contouring the outside of the block. Then drill the hole after probing your datums.

Does anybody else do this to hold super close tolerances on positions and profiles?

I've had to do this once for a part with a .001 profile but used a 3D Haff and Schneider indicator rather than a Renishaw probe. How would you go about doing a probing cycle mid machining to reestablish your G54? Would you have to do macro programming and/or use G92 datum shift? Is there such thing as G92 datum shift?

Thanks,

Chris

 

[???]

I had exactly the same problem. My solution was to measure my cutters and clock them in the holder. I found my cutters are all undersized by 0.03mm. I program all my jobs using the true cutter size which results in the datum and other features being in the correct position.

 

[Mtndew]

Most endmills are ground .001" undersize

Most GOOD end mills are ground to an H6 tolerance.

 

[camhead420]

Most endmills are ground .001" undersize

This is new, I have never heard of such a thing.

 

[daringwilliams]

I've consistently found even high quality endmills etc are about .001" under, not the shanks themselves but the cutting edges, this is so you can adjust them in

My method(s) to suggest would be to do Rough / Semi / Probe / Finish approach where you have a dedicated rougher leaving something like 4x stock to leave, then Semi with a different tool, leaving 2x stock to leave on the feature tolerance, Probe to see if your current Semi cut strategy will hit that final number, then have automatic Length / Dia wear adjusted at control to do Final passes within that Probing cycle

I work with alot of 3d printed metal parts with aerospace type tolerances and parts can have a lot of variability compared to billets etc, this approach works great

Once you have a primary feature in tolerance like a Datum A, you can probe that as a "new" G54 and base all other features on it etc

Position tolerances like that are hard to maintain, so you will need high quality machining centers, repeatable conditions (warmup cycle, including all axes motion, temperature stability, calibration checks at regular intervals possibly between parts)

 

[Matt@RFR]

Making your block dead nuts on size solves your problem.

 

[dandrummerman21]

A question related to your datums.

For your theoretical (or real?) part that you are talking about, since you are locating the hole in the center of a square, can you make B and C the centerline between the surfaces of the square? I understand that there are reasons you must make it an edge, but in lots of cases, I see drawings where a hole just must be centered tightly between two flats, and not necessarily tight to one edge or the other.

As for a cutter ground under, and theoretically being oversize once you cut, that's what cutter comp is for.

Are you the one who will be making this widget? Or is your question just related to how another machinist will have to hit your tolerances that you're putting on the print?


I am running a part with .001 true position and I am cutting all 3 edges, kinda similar to your part but not really. I'm doing it on an HMC. So what I've done is leaving a positive cutter comp value for the finish endmill, run the hole part, then have the machine probe the hole and surfaces and see where I'm at, size and location-wise. Then adjust the cutter comp so my size is perfect and so is my location.

I don't think you really need to update G54 or another coordinate with your probe, but you can update a cutter comp value to make it cut more or less, in process (or manually), as needed.


EDIT: I read the original post wrong, I thought you (the OP) were DRAWING the part, not making the part. My opinion/suggestion above regarding centerline still stand, but if you can't change the print, then just live with it being from the edge and comp it in.

 

[SeymourDumore]

Making your block dead nuts on size solves your problem.

^^^This^^^
If hitting a .001TP is your goal, machining the outside of the block ( your datum ) to size is the absolute easiest to achieve.
As far as probing, I don't see why would anyone probe features that are machined at the same time in the same setup, perhaps even with the same tool.
For size? Absolutely.
For location? That doesn't make sense.

 

[mhajicek]

As said above, comp the cutter in until your periphery is dead nuts. Modern, quality, solid carbide endmills on a decently rigid machine will skim a tenth if you tell them to, or sometimes less on a skim pass; ignore anyone who talks about "rubbing". I can get zeros out to five places on my Mitutoyo mic working with a Haas if I take some time and try.

 

[couch]

.001 TP is not the same as +/-.00035

Can you show us a redacted copy of the print showing -B- and -C- ? Are the Datums being called straight in line with the dimensions or extended past the dimension? This makes a huge difference.

 

[crossthread82]

Comp the endmill in so the part cuts to size, then put the hole in the middle. Done.

Does the TP call out have a modifier? LMC, MMC?

If the -B- and -C- are called out in line with the width dimensions then they are relative to the feature centerline so a hole in the middle of your .002" bigger block would still be within the .001" TP call out, assuming the .002" oversize is within the allowable tolerance of the widths called for -B- and -C-.

 

[D Nelson]

Comp the endmill in so the part cuts to size, then put the hole in the middle. Done.

Does the TP call out have a modifier? LMC, MMC?

If the -B- and -C- are called out in line with the width dimensions then they are relative to the feature centerline so a hole in the middle of your .002" bigger block would still be within the .001" TP call out, assuming the .002" oversize is within the allowable tolerance of the widths called for -B- and -C-.

Start out by using the center of the block as zero that helps 50 percent right there then dial in the Endmills
Don