What's new
What's new

Holding .0002" position between bored holes.

Ukraine Train

Cast Iron
Feb 10, 2014
I'm trying to come up with an approach for this. It's a stainless steel weldment, about 12" long x 6" wide. I will need to put in the 3.5" hole on each end, starting from solid. The hole size tolerance is .001" total and the two need to be located within .0002" of each other on center. I'm thinking I can rough one hole, flip the part, rough the other, then in the same setup run a long boring head through both sides. Is there a better way? Or am I better off getting this ground to size? 2 tenths seems awful tight even in a rigid setup.
Seems like an automotive shop that does line-boring or line-honing would be able to do it easier, unless you're going to build a lot of these. Rough it in for them and let them finish it. Check how much they want you to leave in the holes.
This is a job for jig grinding. however holding .0002 hole concentricity seems very demanding for a weldment. Is the part to be stress relieved before finish machining?

Additionally, how are you going to verify .0002 position on the holes when you (presumably) do not have any ground surfaces to reference?

Would be interested to learn more about this part.

BTW, I have a jig grinder and am in SE Michigan...
Agree with the above. A weldment will definitely move around a lot. A month after the machine work, it is a stretch to think they will still be correct.
To my way of thinking, if the tolerance on the hole is .001", then the misalignment tolerance is undetectable until it exceeds .001"
How ya gonna measure it when you get done? Just clamping it down is going to have an effect on things.
You might consider line honing the bores as well as line boring them. If you have to locate them to a datum as well as to each other, then jig grinding is the way to go.
you may have a chance without the word weldment. with a weldment alignment that tight IMHO is a pipe dream. If they can't measure it better than you can I'd just machine from each end.
My first thought on a part like that is "how in the world are they going to check it?!" You have a small land on each end that they are going to use to establish a ceterline that they will then use to corroborate the results of the C/L of the hole on the opposite side?! You've got to be kidding?!

The cmm operator is going to pick up the hole on one end - then the hole on the other end - then say put a C/L through those two centers and compare it to something else - and then use that comparison to say whether or not your holes are in alignment.

You could end up in a real running battle on this job jut with the interpretation of the cmm results whether the bores are aligned or not.

In all reality, those bores could be out .001 - .002 and a ground bar would still go through them.

Now if there was a 3rd wall with a bore in between the two outside bores it would be a totally different story.

Just work it as close as you can - I am sure it will work.

Data for your customer: steel moves 3 microns per degree foot

Therefore, if you have two holes 12" apart, the difference between those holes will be 0.0004" between the temperatures of 72 degrees Farenheit and 75 degrees Farenheit. This is twice your indicated tolerance. What is the temperature of the room you are in now?

The welding is where it starts to get hilarious.
I shot off an email to verify the tolerances. They also want .0005" profile tolerance of the machined flat surfaces after welding so I think this maybe be a bit over-engineered. I believe the bores will have bearings pressed in so I can see the need for holding alignment but not to this degree.
If it was a stable part this could easily be done on an ID grinder. I have a heald grinder with a red head spindle made just for that. This a very long version of one:

Heald Red Head Internal Grinding Spindle | eBay

Notice that there are bearings right by the grinding wheel and the hole unit goes through the part. Minimum size for this is 3 inch bore so you would be fine.

However I often grind parts like this with the same position specs but also .0003 tenth size tolerance and shoulders. Where I can't use the longer spindle and have to flip the part. This is how I do it: Grind one bore, also grind the face. Flip around and put the ground face on a fresh mag chuck. Then indicate in the ground bore or other reference surface and grind. You have to be careful but .0002 is obtainable with a good grinder and a careful operator.

If this came into my shop I could do the job on my ID grinder, jig grinder, or hone. ID grinder would by far be the fastest and cheapest. If you had a ton of them honing might be on option but if I were you I would be looking for an ID grinding shop. I only jig grind things this big if I can't spin them on the ID grinder.
Part may be a little out of balance to spin on a chuck looking at is again. Though id grinding the thing can spin real slow... I would still probably try it first. Could probably hold it in a 4 jaw just fine if the mag chuck was too sketchy. However then I would only grind one bore at a time and flip it so I did not distort the bore with the chuck.

That size tolerance it would easily be done by someone with a good horizontal boring mill.
Do you already have the job or are you quotin' it? I'd pass. I hate doing over engineered work. Over engineered work usually lends itself to under qualified engineers. Excruciating to work with. And if you ain't passin' on it, you better be gettin some huge margins on work like this.
I shot off an email to verify the tolerances. They also want .0005" profile tolerance of the machined flat surfaces after welding so I think this maybe be a bit over-engineered. I believe the bores will have bearings pressed in so I can see the need for holding alignment but not to this degree.

We do parts not too dissimilar to this to comparable tolerances, though yours are certainly at the tight end.

We do it with weldments made here, too. Perpendicularity and parallelism in the tenths over 20" is not unheard of. Good stress relief and some indicators on the part when you're clamping it in place to ensure it doesn't move during setup. I know I couldn't do it. I'm happy to work with a great bunch of guys.

Every time a thread comes up with tight tolerances, people love to chime in like they're the only ones who know material moves when the temperature changes. Ignore it. There are standards for inspection for a reason. If your customer is going to check it at 20C, do the same. Make sure it has adequate soak time in the climate controlled room. If your customer is going to check it at 85F then find a way to make that happen, too, I guess. Hopefully they're sticking with standard and assuming 20C inspection environment.

You're certainly in a 'line boring' situation, though, unless your HMC table is just fucking phenomenal at re-positioning accurately. Maybe it's good enough. If you can get a bar through it from one setup and still hold the diameter, though, that'd be baller. Otherwise it might be an operation to sub out to a specialty shop.

Those ID grinders are neat as hell.
Hello Ukraine Train,
The two holes that you will produce will be on the same exact centerline, your job is to true-up the 2 datum surfaces that locate the bores. If it were me, I'd 4-jaw chuck and bore this part on a lathe.
In a long, roundabout way, I think they are trying to suggest to you to align bore it, without TELLING you to align bore it. Disturbing the setup would make it near impossible to match up the centerlines.