Hitting datums on the mill

[cgrim3]

Hi all,

Please excuse my naivety. We do mostly lathe work with 2nd, 3rd, and 4th op mill work with a 3 axis vmc. Most of our work is not mill work, mostly lathe work. Most of the drawings we work with have GD&T that is incorrectly applied. We use a haff and schneider 3D probe. We do not have a renishaw probing system.

I understand that a lot of the aerospace/defense work uses GD&T pretty extensively. We have done occasional defense/aerospace work. I know GD&T fairly well and how to interpret it. What I am not familiar with is renishaw probing.

My question is about hitting datums on a 5 axis mill. See below:

Say you have a hole. The surface at the top of the hole is datum A (primary datum), the side of the part is datum B (secondary datum), and the other side is C (tertiary datum). According to the GD&T 3, 2, 1 rule - the primary datum is 3 points (forms a plane), the secondary is two points, and the tertiary is 1 point.

So, do you probe the datum A 3 times to form a plane, datum B twice, and datum C once? Or do you just probe the part like this during inspection on the CMM and not on the mill during machining? When adhering to datums in the feature control frame for the hole, what is the process for probing your parts before machining features (such as a hole) to hold the true position tolerances?

Thanks,

Chris

 

[cgrim3]

Also, I wanted to share a good example of hitting your datums. Not necessarily including the 3, 2, 1 rule but just hitting your datums.

There was a time where we had to machine a simple rectangular block with a pocket going through the middle of the front surface of it. The pocket was half of a tapered cone...the radius started out big at the top of the block and then tapered down to a smaller radius at the bottom of the block. Imagine half of a tapered cone milled into the front surface of a simple block. The cone itself had a surface profile tolerance of .001 relative to 3 datums. One of those datums was the front surface of the block and the other datum was a theoretical plane going through the middle of the part and the cone (front to back). I think the other datum was the top surface of the block. This datum scheme tied the cone up so if a perfectly machined cone was shifted just a tiny bit from center of the block left to right or front to back, it would have blown the profile tolerance. As a note, the overall length and width tolerance of the block was +-.005.

You go to machine the part. Say you programmed the G54 origin (x0, y0, z0) at one of the corners of the raw material and machined the entire block and cone on a 3 axis mill with a bullnose endmill. It is a very good chance that the cone will be out of tolerance. To machine the part, we first had to machine the basic block to within size (size tolerances of +-.005). Then we had to pick up the front surface of the block and set that as Y0. Pick up the Z just by zeroing off on the top. To pick up the X, I wanted to hit the theoretical midplane datum, so I probed the left side and right side of the block and split that number in half to find the center of the block and set that number as my X0. Basically zeroing my axes on the datums on the print. We machined the cone pocket and it was within the .001 surface profile tolerance.

The fact of the matter is, if the cone was shifted left to right along the front face of the part just a couple tenths, it would have thrown the profile out. If the cone was shifted front to back a couple tenths along the centerline of the part, it would have thrown the profile out.

It seems like with GD&T, the only way to really succeed is to always hit your datums. Maybe not use the 3, 2, 1 rule. But I suppose it's always important to hit your datums.

But for sure people or shops not used to GD&T, they would struggle with this part. Hell, we scrapped this part once trying to make it because the cone was so tied up with the datums and surface profile and the fact that the overall size of the block could vary +-.005.

Does everyone else here approach these jobs the same way? Does anybody else do it differently or hit your datums differently? Anybody use the 3, 2, 1 rule when hitting your datums using renishaw programming on say DMG 5 axis machines?

 

[vmipacman]

Did you get a cmm QC report on your final part? Have they QCd it yet and paid the bill? Sounds like you did well on a weird tricky part.

 

[cgrim3]

yeah we got the CMM QC on the final part and it passed. It was a tricky part. We scrapped one part trying to get there but I got it on the final attempt. The fact that the overall length and width size tolerance of the block is +-.005 is misleading because you think you have a wide open tolerance there. The fact of the matter is, no matter the length of the block, the cone had to be placed dead nut in the center or the profile would be out. Goes to show that you have to hit your datums before you do any machining.

Regardless, anyone here apply the 3 2 1 rule to their renishaw probing cycles?

 

[Dan from Oakland]

The problem you will find with probing is the probe only measures the points it hits. The deffn of a datum for GD&T purposes is a gage perfect surface for your B datum example above. In reality this might be the stationary jaw of a vise. When you push your part up against that surface if your part surface is "lumpy" , the part contacts the reference surface on its high spots. But if you probe that same part surface, you may not be probing those high spots. How many folks probe the vise jaw rather than the part surface?? Probably a crappy descripton on my part, but hopefully you get the idea.

 

[007Rob]

yeah we got the CMM QC on the final part and it passed. It was a tricky part. We scrapped one part trying to get there but I got it on the final attempt. The fact that the overall length and width size tolerance of the block is +-.005 is misleading because you think you have a wide open tolerance there. The fact of the matter is, no matter the length of the block, the cone had to be placed dead nut in the center or the profile would be out. Goes to show that you have to hit your datums before you do any machining.

Regardless, anyone here apply the 3 2 1 rule to their renishaw probing cycles?

Just to give you another perspective, if you made this part leaving the outside on the + side of the tolerance and CMM results ended up with the profile being slightly shifted, could you use the CMM report to tickle one of the sides the bring the profile in?

ie. you could think of the extra material on the sides as room for "adjustments" after the tricky part is done.

 

[cgrim3]

Yes I could've done that to bring the cone within tolerance. However, if the cone was off from front to back, there wasn't much I could've done.

 

[cgrim3]

Do not many people use renishaw probes and apply the 3, 2, 1 rule (primary datum 3 points, secondary datum 2 points, and tertiary datum 1 point) to their probing cycles?

 

[motox2121]

Do not many people use renishaw probes and apply the 3, 2, 1 rule to their probing cycles?

I am interested as well about the workflow with probing at angles other than A0 / B0 / C0. Apparently my haas cant do this with Dynamic work offsets. But manually it works. From another programmer I spoke to, he said he manually jogs to the correct index angle, then probes XYZ. The cam software outputs the correct a / c #'s automatically.

This is something that I have asked a lot of people out but haven't heard many good technical explanations on how to approach this - for me specifically on the 5 axis side.

 

[cgrim3]

I am interested as well about the workflow with probing at angles other than A0 / B0 / C0. Apparently my haas cant do this with Dynamic work offsets. But manually it works. From another programmer I spoke to, he said he manually jogs to the correct index angle, then probes XYZ. The cam software outputs the correct a / c #'s automatically.

This is something that I have asked a lot of people out but haven't heard many good technical explanations on how to approach this - for me specifically on the 5 axis side.

I take it that by not many replies, not many people use the 3, 2, 1 GD&T rule on their probing cycles on 5 axis machines. I know of one shop currently doing it but was wondering if a lot of shops on here were doing it

 

[couch]

I take it that by not many replies, not many people use the 3, 2, 1 GD&T rule on their probing cycles on 5 axis machines. I know of one shop currently doing it but was wondering if a lot of shops on here were doing it

For first op stuff there’s really no need to be doing that much probing if all five sides are being cleaned up.

On second/etc op stuff most will typically be built into the workholding. 3-2-1 isn’t really for probing, it’s for degrees of freedom elimination which is more often than not taken into account within the workholding itself.

Also, the number of points taken is going to heavily depend on what the features/datums are in the feature control frame. A cylinder for example might be more than six points to align it.

GD&T isn’t there to dictate how to manufacture or measure a part, it’s there for dimension/tolerance clarification and orientation precedence when laying out a part for inspection. Of course datum precedence will be taken into account when manufacturing but it isn’t a standard for manufacturing.

 

[cgrim3]

For first op stuff there’s really no need to be doing that much probing if all five sides are being cleaned up.

On second/etc op stuff most will typically be built into the workholding. 3-2-1 isn’t really for probing, it’s for degrees of freedom elimination which is more often than not taken into account within the workholding itself.

Also, the number of points taken is going to heavily depend on what the features/datums are in the feature control frame. A cylinder for example might be more than six points to align it.

GD&T isn’t there to dictate how to manufacture or measure a part, it’s there for dimension/tolerance clarification and orientation precedence when laying out a part for inspection. Of course datum precedence will be taken into account when manufacturing but it isn’t a standard for manufacturing.

This information here is great. Thanks. This is exactly what I was looking for. Thanks man

 

[rjwalker1973]

Also, I wanted to share a good example of hitting your datums. Not necessarily including the 3, 2, 1 rule but just hitting your datums.

There was a time where we had to machine a simple rectangular block with a pocket going through the middle of the front surface of it. The pocket was half of a tapered cone...the radius started out big at the top of the block and then tapered down to a smaller radius at the bottom of the block. Imagine half of a tapered cone milled into the front surface of a simple block. The cone itself had a surface profile tolerance of .001 relative to 3 datums. One of those datums was the front surface of the block and the other datum was a theoretical plane going through the middle of the part and the cone (front to back). I think the other datum was the top surface of the block. This datum scheme tied the cone up so if a perfectly machined cone was shifted just a tiny bit from center of the block left to right or front to back, it would have blown the profile tolerance. As a note, the overall length and width tolerance of the block was +-.005.

You go to machine the part. Say you programmed the G54 origin (x0, y0, z0) at one of the corners of the raw material and machined the entire block and cone on a 3 axis mill with a bullnose endmill. It is a very good chance that the cone will be out of tolerance. To machine the part, we first had to machine the basic block to within size (size tolerances of +-.005). Then we had to pick up the front surface of the block and set that as Y0. Pick up the Z just by zeroing off on the top. To pick up the X, I wanted to hit the theoretical midplane datum, so I probed the left side and right side of the block and split that number in half to find the center of the block and set that number as my X0. Basically zeroing my axes on the datums on the print. We machined the cone pocket and it was within the .001 surface profile tolerance.

The fact of the matter is, if the cone was shifted left to right along the front face of the part just a couple tenths, it would have thrown the profile out. If the cone was shifted front to back a couple tenths along the centerline of the part, it would have thrown the profile out.

It seems like with GD&T, the only way to really succeed is to always hit your datums. Maybe not use the 3, 2, 1 rule. But I suppose it's always important to hit your datums.

But for sure people or shops not used to GD&T, they would struggle with this part. Hell, we scrapped this part once trying to make it because the cone was so tied up with the datums and surface profile and the fact that the overall size of the block could vary +-.005.

Does everyone else here approach these jobs the same way? Does anybody else do it differently or hit your datums differently? Anybody use the 3, 2, 1 rule when hitting your datums using renishaw programming on say DMG 5 axis machines?

Now go find the engineer that toleranced that part and hit him with a hammer. As to your original question . If you are probing a datum that is not going to be machined, as in there is no material to be machined off, I always indicate my edges straight before probing and probe multiple spots along the edge or edges. If you have enough material to mill the edges it makes that a lot easier because you are not having to dial the program in to a finished edge. I use the 3,2,1 rule when I probe my parts . It is just more accurate.

 

[EricGushiken]

cgrim3, since surfaces are being called out as datums, ideally, you would need to probe however many times along each surface in order to give you reasonable confidence that you picked up the 3 highest points on datum feature A, the 2 highest points on datum feature B, etc.