I have a customer who needs me to hold a .0005 tolerance ID on a part made with C12L14. I’ve been having trouble getting the tolerance close enough on my 6 spindle Acme bar machine. I’ve been trying for days to ream it up to specs, but I’ve never had to go this close before and I’m starting to run out of patience. Are there any tricks to getting the tolerance right.
Shop Doc Forum » Screw Machine Issues
trouble getting close enough tolerance on Acme using C12L14
(7 posts) (7 voices)-
Posted 2 years ago #
-
There is a technique, which may help you hold your tolerance on the part, known as ballizing. It can actually give you tolerances as close as .0001-.0002. Ballizing isn’t anything new, but usually it is utilized after machining, when you have a ball that you press through a through-hole to size the ID.
What you can do is this. First, ream your part the best that you can, and then afterward, silver solder a carbide ball to the end of a shank and put it in one of your open spindles—probably your fourth position spindle on a six spindle acme. At the same time, for this to function properly as you’re sealing everything off, you will need a little hole that will go through at an angle that doesn’t interfere with the OD of the part, to let air behind there escape as you’re ballizing the part. Then run your operation. It’s just in and out, so it doesn’t limit your cycle time of making the part. You can now complete the part on the screw machine and hold a very close tolerance, usually getting better than a 10 - 6 micro inch finish on the hole.
Things to remember
The balls are made of carbide, so you will have to experiment a little bit with size because what you’re really doing is displacing material, and it will spring back. So if you would have to hold, for example, better than a half a .0005 tolerance, then you will need to experiment with two or three different balls to find the result you are looking for. Also, like anything, the balls are only as good as how close you ream. In other words, the reamed hole would need to be held close to keep consistency on the ball that you’re working with. They both work a little bit together. So if you had a hole that was varying .002 before you ballized it, I still think you could ballize it and hold it within .0005. If you wanted it any closer, you would probably have to ream within .001. Then, I think you would be able to hold within .0002 or better. Also, you need to make sure that the same type of gauging you are using, your customer is using.Good luck
Posted 2 years ago # -
This also sounds like it could be an ideal candidate for honing. While it probably means having someone outside your shop doing the final sizing, it might be better than fooling around with this for days. This is percisely (pun intended) The kind of work we do for lots of customers.
Posted 2 years ago # -
I'm no expert on reaming, and not even sure what a 6 spindle acme bar machine is. But I know .0005 is not outrageous for a reaming operation. What is the size of the hole you are reaming to? What length reamer are you using? (Longer shanks self align with the pilot hole better when you have tiny misalignments between tailstock and headstock.) Is the collet or chuck holding the part and the collet or chuck holding the reamer clean and burr free? Is the reamer shank smooth and concentric? Is the reamer ground properly? Is the the reamer online with the headstock? Is sufficient coolant applied to prevent the reamer from heating up and cutting oversized? Is the pilot hole large enough that the reamer will not be overloaded and cause chips to pile up in the flutes? Or is the pilot hole so large that the cutting lips of the reamer have no support during the cutting operation?
Posted 2 years ago # -
I don't know this type of metal, or how deep the hole is, whether it's blind, but I've been able to hold .0002 with a nice rigid boring bar in a variety of stainless steels and other metals. I had a job in cupronickel from bar stock that ended up with a .002 wall, where by the +/- .001 tolerance it could vanish and still be in tolerance. We held .0001 id and od by using 2 tools, one inverted for the od and normal for the id in one pass.
If the hole is long and deep then honing or ballizing are good choices. Think peaks and valleys in the finish. With ballizing the peaks are pushed into the valleys.
TomPosted 2 years ago # -
First you must make sure your drilled hole is holding to a tight spec before the reaming will hold. I'm not a big fan of bought reamers--Sounds like you need a good shop made carbide flat reamer or drill to hold that tight.
TRRPosted 2 years ago # -
our guys just grind some of the reamer flutes off.. seems to work. too many flutes build up and force the reamer to one side or other. try two or four flutes, else have an odd number, like 3. seems to work on ours.
RayPosted 2 years ago #
Reply
You must log in to post.
