Need ideas fixturing, holes true position +-.0005

[EPAIII]

Aluminum part
All sides finished
Two holes drilled/bored
No mention of any coolant being used

And you are probably doing those operations one after another, as fast as you can. Making heat. Aluminum expands.

I could be wrong, but I just wonder if you might be better off doing the operations one at a time, giving the parts time to cool off between them. Or use flood coolant. Or both.

Make one or more extras. Check the dimensions produced by each operation on the first part of the batch and then adjust as needed for the remaining ones.

 

[Dan from Oakland]

True Position is NOT a +/- feature- the center line of your feature needs to be located within a .0005" diameter circle
of the basic dimensions locating the tolerance zone. (assuming here a circular tolerance tolerance zone.) This is pretty basic GD&T.

 

[plastikdreams]

 

[CarbideCarGuy]

I may not be understanding something from the first post. Why are you not machining the holes at the same time you cut the profile?

That is what I would like to do. There is no way to hold the part if I want to machine all four sides AND the holes in one operation. That is my original question, how would I hold this?

I'm certainly not a "tolerancing" authority, but I'm pretty sure that True Position Error tolerances are properly expressed as magnitudes, not plus-or-minus values.

If my belief is correct, the method of reducing the measured locations of the holes to derive and evaluate the actual True Position Error needs to be reviewed and, if necessary, corrected.

You are correct. My mistake, it is TP of .0005, no Max material (or M with a circle around it)

You don't say how old your machine is, or how hard it's been run. If it's old and worn, you can pretty much forget it. If it's young and fresh, it can be done:

First thing I would do is have the machine laser calibrated. I have Productivity Quality do mine, costs about $1500 IIRC. They map the errors in the machine and adjust the compensation tables in the control. You also need a very consistent ambient temperature in the shop, so the machine doesn't grow and warp with temperature changes; plus or minus a degree or two is ideal. No direct sunlight hitting the machine through windows. Then you should at least have consistency, with a decent setup and torque wrenches. If you can get a consistent result but it's out of tolerance, then add Kentucky windage (fudge factors) in your program to bring it in.

If you have multiple different machines, run the tight tolerance stuff on the smallest machine that will fit the part (provided it's of suitable quality); smaller machines have less thermal growth.

It is a 2021 Haas VF2SS. I don't have the means to calibrate it with lasers, I asked my local Haas retailer to send a service guy to calibrate for backlash or any errors. They said the machine is spot on already. The shop isn't exactly ideal, the machines near a bay door, the boss likes to crank the heat in the morning. I used torque wrenches and found the sweet spot of tightening without warping the part, etc.

One important feature you haven't mentioned is distance between holes. Aluminum moves .0012" in 10F in 10 inches. I can hold a part in my hand and make it move out of tolerance.

I don't mean to throw shade on your machinery, but I wouldn't trust a CMM in a shop that uses Haas machines for any +-.0005 features. +-.002, yea, maybe. Run your part across the CMM 4 times, each time reorienting the part 90 degrees, and, if possible,4 different operators. Tell us the spread on your measurements.

I know you want to do the job in house. I understand, I get it. But if you don't have the equipment both you and your customer end up mad. Everybody loses all around.

I believe it Could be done but the CMM operator doesn't adopt new techniques very well so I have to setup my machine to compensate his style... If catch my drift... I made the part slowly to I don't think heat is the issue, and then we let it acclimate in the inspection room before it's checked. I am the only operator/setup/programmer and this is our only milling machine. We have two other lathes but I can only run one machine at a time, considering it's all small lots. This plate was only 2 pieces. I ended up making 6 of them just practicing, then the welder messed all of them up anyway. so there goes all my hard work.

I also don't understand the +-.0005 true position. What is the TP actually? If the TP is .001, the most both axes can be out at the same time is .00035. If the TP is .0005 that error is reduced to .00017. Pretty close! How close is your CMM? And how consistent is the temperature of everything?

Either way, if you are establishing the outside of the part during the boring operation that adds another level of uncertainty to the problem because the datum surfaces can move about.

Try leaving the finished part in the vise and go to position and indicate each hole. If it is not dead on there is one problem. Then take that part out and put it back in the vise. Re-indicate each hole. If they are not dead on again you have a clamping repeatability issue. If you don't have repeatability you're just chasing your tail. Are you chucking on an unfinished surface? Does your cmm measurement repeat?

I'm just amazed you can hold .0001 total on the diameter without any trouble. How the heck are you measuring that?

TP of .0005. I would like to machine all sides and the hole in one shot. My original question was how to hold it. I tried doing something similar where I would indicate the piece straight and flat at a torque that wouldn't warp the part, i think it was somewhere around 10ft/lbs. I would indicate it, and remove it and repeat with different torque values until I discovered the sweet spot. In the past, i've checked hole diameters with an air gauge but this place doesn't have one, they are checking it with the CMM.

Is there a M with a circle around it on the print in the box with the true position indicator? If so there may be bonus tolerance allowed. For any given hole, the bonus tolerance is equal to the actual size of the hole minus the smallest size of the hole.

I hate true position, it's gotta be the dumbest thing in gd&t. Especially when they use unrealistic tolerances.

There is no M for this feature. Even if there was, an extra .0001 wouldn't help that much. I also hate true position. I understand the need but I also think .0005 is way too tight.

Aluminum part
All sides finished
Two holes drilled/bored
No mention of any coolant being used

And you are probably doing those operations one after another, as fast as you can. Making heat. Aluminum expands.

I could be wrong, but I just wonder if you might be better off doing the operations one at a time, giving the parts time to cool off between them. Or use flood coolant. Or both.

Make one or more extras. Check the dimensions produced by each operation on the first part of the batch and then adjust as needed for the remaining ones.

We use flood coolant, xtreme cut 250. It is a two piece lot and takes about ten minutes a piece to setup, then I let acclimate. The operations are separate, finishing the sides first, then the holes.

 

[TeachMePlease]

You're holding .0005" TP on a hole... And then they're going to a welder?

Seems like this might be a design issue...

 

[CarbideCarGuy]

You're holding .0005" TP on a hole... And then they're going to a welder?

Seems like this might be a design issue...

I know, I don't design the part, I just complain about them...
The .0005TP is to locate a pin into another hole on a mating part. The two parts get welded, the pins removed then another hole machined after welding that has to match the opposite end which has the same process. The hole after machining has a TP of .0200"

I don't understand it but they were not willing to budge on the tolerances or design.

 

[teemfan93]

I know, I don't design the part, I just complain about them...
The .0005TP is to locate a pin into another hole on a mating part. The two parts get welded, the pins removed then another hole machined after welding that has to match the opposite end which has the same process. The hole after machining has a TP of .0200"

I don't understand it but they were not willing to budge on the tolerances or design.

I'm sorry in advance if I don't understand the workflow or design. Could you do the first hole (for the two parts with welding/pin) undersize on the diameter, and then post machine to final size after the fact? I am thinking of a similar workflow to match drilling. You undersize the holes you need until the parts are mated, then drill/finish to final tolerance/diameter.

 

[CarbideCarGuy]

The pin is to align the parts for welding. Machining after welding would defeat the purpose. I hope this helps to visualize the part and features without giving away too much
EDIT: so I took all this time to "Draw" the part with characters in text form and it removed all the spaces and looks terrible so I screen shot and attached it as well as leaving the original for reference.

This is what the left and right plate look like:
| |
| |
| O O |
This is what the bottom plate looks like on both sides:
_____________
| O O |
Then two pins get pressed in then welded

| | | |
| | | |
| | \ <Welds> / | |
| | \ / | |
Pin> | | | | <Pin

Then the pins get removed and a new holes machined on top must line up within .02" TP:
New>| | | |<New
| | | |
| | \ / | |
| | \ / | |
| | | |

 

[mhajicek]

That is what I would like to do. There is no way to hold the part if I want to machine all four sides AND the holes in one operation. That is my original question, how would I hold this?

It is a 2021 Haas VF2SS. I don't have the means to calibrate it with lasers, I asked my local Haas retailer to send a service guy to calibrate for backlash or any errors. They said the machine is spot on already. The shop isn't exactly ideal, the machines near a bay door, the boss likes to crank the heat in the morning. I used torque wrenches and found the sweet spot of tightening without warping the part, etc.

You might be able to hold the part on a vacuum fixture. I have a Pierson's that I like. Either gasket around where the holes go, or leave a .005" skin on the bottom of the hole to maintain vacuum, and take it off when chamfering the backside. Depending on the size of the part (bigger is better for this), you might have to take lighter cuts to keep from shifting the part.

If you can't keep the temperature of the machine constant within a few degrees at most, you can absolutely forget about trying to hold a tolerance that tight, especially over a whole shift or multiple days. I mean you might get lucky, but it would take a lot of luck. Chances are better if you're doing the profile at the same time as the holes, as they're more likely to shift in unison.

Oh, and Haas doesn't do the laser calibration. You need to find someone like Productivity Quality, who did mine. I'm sure they'd fly out to you, but that would jack the price considerably. But that's not going to help much if you can't stabilize the temperature first.

 

[adamm]

Your ascii art is impressive.

 

[the average Joe]

Agree with what everyone else is saying, and if you're not in a climate controlled environment, and the customer is not in a climate controlled environment when they check the parts, then everything goes out the window. You can get to .0002 location accuracy using edge finders and manual milling machines, but stuff like that takes a whole lot of finesse and it's not really something you'd want to do long tern across multiple machinists and shifts. At the end of the day, it also comes down to how the tolerance is interpreted as well.

Try machining a thin part out of a block of PTFE, and see how much you and the client argue over thermal variability and tolerancing.

How is this company checking these parts? Are they even checking these parts?
I have a client who constantly over tolerances parts and we almost always lose on quotes because we have to hold all those numbers they put on the drawing. I found out through other local shops that the "incoming inspection" at this company consists of a single guy with a height gage, 12 inch calipers and a small surface plate. They basically don't check anything and just bolt it all together and the only time that anyone complains is when parts literally don't fit each other. But, it's not like I can just fake it and send them out of spec parts even if they don't really care.

 

[empower]

You don't say how old your machine is, or how hard it's been run. If it's old and worn, you can pretty much forget it. If it's young and fresh, it can be done:

First thing I would do is have the machine laser calibrated. I have Productivity Quality do mine, costs about $1500 IIRC. They map the errors in the machine and adjust the compensation tables in the control. You also need a very consistent ambient temperature in the shop, so the machine doesn't grow and warp with temperature changes; plus or minus a degree or two is ideal. No direct sunlight hitting the machine through windows. Then you should at least have consistency, with a decent setup and torque wrenches. If you can get a consistent result but it's out of tolerance, then add Kentucky windage (fudge factors) in your program to bring it in.

If you have multiple different machines, run the tight tolerance stuff on the smallest machine that will fit the part (provided it's of suitable quality); smaller machines have less thermal growth.

another thing to consider as well is that 6061 is gonna move as well, are you able to use cast aluminum tooling plate instead of 6061? will be a lot more stable.

 

[empower]

I know, I don't design the part, I just complain about them...
The .0005TP is to locate a pin into another hole on a mating part. The two parts get welded, the pins removed then another hole machined after welding that has to match the opposite end which has the same process. The hole after machining has a TP of .0200"

I don't understand it but they were not willing to budge on the tolerances or design.

i'd laugh in the idiot's who designed that face.
some people should not touch CAD. move on to a different job, you'll earn nothing but gray hair from this customer.

 

[the average Joe]

Whoa, I missed that the parts get welded. No way all that stuff stays in place once that happens. Whoever designed this doesn't know what they're doing.

 

[guythatbrews]

Agree with what everyone else is saying, and if you're not in a climate controlled environment, and the customer is not in a climate controlled environment when they check the parts, then everything goes out the window. You can get to .0002 location accuracy using edge finders and manual milling machines, but stuff like that takes a whole lot of finesse and it's not really something you'd want to do long tern across multiple machinists and shifts. At the end of the day, it also comes down to how the tolerance is interpreted as well.

Try machining a thin part out of a block of PTFE, and see how much you and the client argue over thermal variability and tolerancing.

How is this company checking these parts? Are they even checking these parts?
I have a client who constantly over tolerances parts and we almost always lose on quotes because we have to hold all those numbers they put on the drawing. I found out through other local shops that the "incoming inspection" at this company consists of a single guy with a height gage, 12 inch calipers and a small surface plate. They basically don't check anything and just bolt it all together and the only time that anyone complains is when parts literally don't fit each other. But, it's not like I can just fake it and send them out of spec parts even if they don't really care.

I used to see this sort of thing a lot more than I do now. I can't compete and don't even try to compete with underpriced shops that don't respect drawing requirements. It's a slippery slope when you head this way.

As you say some customers don't understand what they need. When receiving inspection is, if it works, it works, it's bad for everyone. This type of customer is not my type of customer.

It's easy to check tolerances at quote time. Then I either decline to quote if it's too tight (maybe just too tight for me), or ask a question if something seems odd. I hardly ever question tight tolerances but I do question what might be a mistake.

As a vendor I don't consider it my place to question tolerances. Maybe for a customer with whom you have a good relationship, but It can cause hard feelings.

Edit: I've also bern on the other side of the fence with an impossible drawing thrown in my lap. Tell the higher ups it can't be done they just say do it. Not a great place to be!

 

[empower]

I used to see this sort of thing a lot more than I do now. I can't compete and don't even try to compete with underpriced shops that don't respect drawing requirements. It's a slippery slope when you head this way.

As you say some customers don't understand what they need. When receiving inspection is, if it works, it works, it's bad for everyone. This type of customer is not my type of customer.

It's easy to check tolerances at quote time. Then I either decline to quote if it's too tight (maybe just too tight for me), or ask a question if something seems odd. I hardly ever question tight tolerances but I do question what might be a mistake.

As a vendor I don't consider it my place to question tolerances. Maybe for a customer with whom you have a good relationship, but It can cause hard feelings.

Edit: I've also bern on the other side of the fence with an impossible drawing thrown in my lap. Tell the higher ups it can't be done they just say do it. Not a great place to be!

i remove myself from those situations. shit isnt worth my sanity.

 

[boslab]

From the dungeon of my memory, circle M ( that’s how we used to say it on the phone) is the maximum material condition, for a hole as small as it can be , shaft as big as it gets
Mark

 

[couch]

Without more detailed information on how the datums are called out and how the feature control frames are written, exactly, giving advice on process and workholding is going to be a shot in the dark. Can you post any photos of the section you’re talking about and redact all other info? At least, maybe you have and I missed it, mention how the datums are called. Are the faces, midplanes, other features, etc the datums? You mentioned “all sides”, but this isn’t clear. Is the Position tolerance a composite or are each holes called independently? This all will dictate how the parts should be held and made.

QC’s job is not to tell you how to make the part, regardless of CMM or not. His job is to inspect the part, that’s it. You shouldn’t be working around him. Make it how you think it should be made and inspect it per the guidelines laid out on the print. I can’t even count how many times I’ve checked parts on a plate with gages, properly, and had a CMM guy fail my parts, only to find out his program was bad or his setup was bad or his understanding of GD&T was bad. If you are checking it good, show QC how you are checking it. Most guys that sit in QC never spent time cutting metal. The CMM is not the last word.

 

[rjwalker1973]

I may have missed the answer to this , but how many datums are you holding this TP to? Any more than 1 and it is a crap shoot on that machine to be honest.

 

[rjwalker1973]

From the dungeon of my memory, circle M ( that’s how we used to say it on the phone) is the maximum material condition, for a hole as small as it can be , shaft as big as it gets
Mark

According to where it is in the box. If it is in the first part of the box with the tolerance it is MMC if it is in the datum box it is MMB Maximum Material Boundary.