Need ideas fixturing, holes true position +-.0005

[CarbideCarGuy]

Hello!

I'll jump right into it. I got this job with a true position of +- .0005" on two holes that have a +.0001 -0 tolerance on the diameter.
The machine is a Haas VF2SS with a Saunders Machine Works Fixture Plate. I got 140 degree spot, 135 degree split point drill and my fancy new digital boring bar from Big Kaiser. Holding size isn't the problem. The problem is holding the part correctly to hold position.
I need to machine all sides to finish size and also drill/bore the holes in the same operation. I programmed it to spot, drill, and bore before moving to the home position, then the next hole so any backlash shouldn't be an issue. But it's always .001 or less, out of position. I think it's because I cut the sides, then move it to a vise and drill the through holes. Probe is calibrated and parts indicated but it still doesn't quite reach the tolerance I'm aiming for.
Any suggestions on how to hole a piece of aluminum 6061, to machine all sides (datums) and the holes in one operation. The answer is probably right under my nose but I'm the only machinist here so I have no one to point out the obvious. Thanks in advance

 

[Limy Sami]

Bluntly put, you need a jig borer and not a common or garden milling machine

 

[SIP6A]

Hello!

I'll jump right into it. I got this job with a true position of +- .0005" on two holes that have a +.0001 -0 tolerance on the diameter.
The machine is a Haas VF2SS with a Saunders Machine Works Fixture Plate. I got 140 degree spot, 135 degree split point drill and my fancy new digital boring bar from Big Kaiser. Holding size isn't the problem. The problem is holding the part correctly to hold position.
I need to machine all sides to finish size and also drill/bore the holes in the same operation. I programmed it to spot, drill, and bore before moving to the home position, then the next hole so any backlash shouldn't be an issue. But it's always .001 or less, out of position. I think it's because I cut the sides, then move it to a vise and drill the through holes. Probe is calibrated and parts indicated but it still doesn't quite reach the tolerance I'm aiming for.
Any suggestions on how to hole a piece of aluminum 6061, to machine all sides (datums) and the holes in one operation. The answer is probably right under my nose but I'm the only machinist here so I have no one to point out the obvious. Thanks in advance

I would ditch the vice and fixture plate. You don't say anything about the part but you're probably distorting it from heat and the vice. Get it on the machine table with some precision ground blocks and toe clamps. Your holes are on location in the machine but when you take the part out of the vice its distorting. +- .0005 isn't that tight a tolerance, You could do that in a tight Bridgeport.

 

[plastikdreams]

You are running on the ragged edge of repeatability for that machine. If anything I would see if the tolerance can be opened a little bit, it you are hitting .001 or less see if you can get a few or 5 tenths on it.

Where in North jersey?

 

[eKretz]

How are you checking the hole locations? Need to make sure that it's a repeatable and accurate method. CMM?

To get everything important in one op is a good idea. Do you have any non critical holes that could be put in first for clamping while you do the critical stuff? If so, put those in with the vise then switch to another fixture with full access to the important stuff, using the non critical holes for clamping to the fixture.

 

[Waakzaamheid]

How big is this piece? Is Wire EDM an option?

 

[CarbideCarGuy]

Bluntly put, you need a jig borer and not a common or garden milling machine

Thanks for your input. Unfortunately, I don't have that option and I need to make it work with what I got.

I would ditch the vice and fixture plate. You don't say anything about the part but you're probably distorting it from heat and the vice. Get it on the machine table with some precision ground blocks and toe clamps. Your holes are on location in the machine but when you take the part out of the vice its distorting. +- .0005 isn't that tight a tolerance, You could do that in a tight Bridgeport.

I use a torque wrench to set clamping pressure while watching a .0001 test indicator so I don't deflect. With the .5" thick piece sunk into the vice, I was able to clamp it with .0002" deflection in the z direction. The datum surface is on the fixed jaw, the side datum is indicated straight , shimmed if needed but usually not needed.
.0005" on a positional tolerance doesn't seem like it would be a problem but it's turning out to be a lot more difficult than it seems.

I do like the idea of toe clamps but i still wouldn't be able to machine all features in one Op. Unless I just machine the Datums and holes in one op and save the rest for a second op.

You are running on the ragged edge of repeatability for that machine. If anything I would see if the tolerance can be opened a little bit, it you are hitting .001 or less see if you can get a few or 5 tenths on it.

Where in North jersey?

We asked about the tolerance, it can not be opened up. It's for a pin which locates the plate to another plate which also has a third, identical plate on the far side. It's a test of skill if anything... I am new to programming so I haven't built my fixturing skill yet. I am in West Milford but work a little more south. NJ manufacturing is thriving right now, good to meet a fellow NJ machinist.

How are you checking the hole locations? Need to make sure that it's a repeatable and accurate method. CMM?

To get everything important in one op is a good idea. Do you have any non critical holes that could be put in first for clamping while you do the critical stuff? If so, put those in with the vise then switch to another fixture with full access to the important stuff, using the non critical holes for clamping to the fixture.

We are using a CMM. We recalibrated, tried different methods of checking, etc. I checked it with pins and a drop indicator and it was good but the CMM takes president.

How big is this piece? Is Wire EDM an option?

It isn't big, 6x6x.5" Wire EDM would be an option if we had a wire in house.

 

[BugRobotics]

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?

 

[John Garner]

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.

 

[mhajicek]

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.

 

[gbent]

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.

 

[guythatbrews]

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?

 

[gustafson]

+ a tenth to hold a pin
sigh

 

[plastikdreams]

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.

 

[guythatbrews]

+ a tenth to hold a pin
sigh

I know, right.

Stuff like this I try not to justify the designer's intent. It's usually a forlorn hope. I just don't take the job.

 

[guythatbrews]

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.

With the .0001 total on the hole you'll get a little bonus tolerance.

 

[plastikdreams]

With the .0001 total on the hole you'll get a little bonus tolerance.

Yeah, that's where the unrealistic tolerance comes in lol...especially in 6061.

 

[John Garner]

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

Amen, Brother!

If I had a dollar for every time I needed to explain to a design engineer or Material Review Board why a hole having a location error magnitude between 0.0050 inch and 0.0100 inch violates a True Position Error tolerance of 0.010 inch, I could take plasticdreams, eKretz, and Limy Sami to a steak dinner at a nice restaurant in San Francisco . . . including airfare.

And if I had another dollar for every time I've had to explain to those same people why knowing only the True Position Errors of two holes doesn't provide enough information to determine if the holes are too close together or too far apart, I could spring for Business Class tickets.

 

[plastikdreams]

The best is when you ask the designer to explain true position and he says oh I've seen it on other drawings so I just put it there.

 

[boslab]

I can, slowley with toolmakers buttons, and I mean slow!
Mark