How can I eliminate side play in PM940V quill?

S

scattermaster

Registered
Registered
Joined
Jun 19, 2017
Messages
83
SO,
I've had my PM940V for a few months and it performs great as long as I'm not trying for tight tolerances. Now I have a need to tighten up my game and I don't know how...
At this point i believe that free play in my quill is my biggest problem and I don't know how to reduce / eliminate it. I verified side play with a dial indicator.
My symptom is this. If I drill and ream a 1/2" diameter hole. Remove the tooling and install my dial test indicator, it says I'm not over the hole. My X and Y are locked down and my DRO has not changed. The indicator says I'm pretty good in the Y direction but out by as much as .002" in the X direction.
If I bore the hole after drilling it gets better but not perfect.
My goal is to do some production work and I won't have time for boring the holes. I need to be able to do this by drilling and reaming.
What are your thoughts?
Is there a way to adjust the bearings in the quill and reduce the side play?
thx,
Jim
 
without knowing how much side play you are talking about, it might be well within manufacturing tolerances. The common way of tightening up the quill, is to add a little drag by very lightly locking the quill.

More importantly drilling and reaming is not the best way to get an accurately positioned and sized hole. Even good drill bits can walk, thus they can't be trusted when tight positional tolerances are needed. A reamer will follow the pre drilled hole, so if its its out of position the reamed hole will be as well.

Assuming you aren't using any exotic tooling, the steps to get an accurately positioned and sized hole are as follows.
  1. Drill an undersized hole.
  2. Bore the hole slightly undersized. (boring ensures the hole is accurately positioned within the limits of the machine.
  3. ream the hole to final size.
 
I don't remember the source, but I have seen someone demonstrate how drilling progressively larger hole in rather small steps gets you a hole very close to nominal and very round in shape. You can ream that and call it good.

Going straight to a large diameter drill and pushing it through will get a you a hole faster, but quality/accuracy/precision would suffer.

I would try the small steps approach before messing with other stuff, unless you are a legit production shop and time is actually money.

cheers,
wm_crash
 
You did not mention how thick, another thing I was thinking about is using an annular cutter instead or a drill, or a step drill?
 
Ok,
I'm working with cast iron hydraulic pump housings. (ductile iron maybe?)
The existing holes are 12mm diameter and 13mm deep. 180mm spacing on centers. I don't have a tolerance for that spacing but my experience tells me that I have have to be within 3 or 4 thou between the pair. So theoretically I could be .002" off center on both and still be in spec.
I want to be inside of that.
The new holes are 16mm diameter, -.000mm +.018mm. (.6299"-.6306" for a .0007" tolerance) with a 15.5mm depth at the bottom corner of the hole. (not the center)
The pins that go in the holes are 16.023mm-16.034mm. I measured 2 samples and they are right at .6312" dia. (16.0324mm)
I think I should shoot for the large end of the tolerance on my holes.
My customer is needing 4 of these per day and there is also another piece that has to be done as well. So, yeah it's a production run and I'm concerned that boring will eat up too much time.
Possibly I could get my boring head set to achieve the perfect diameter and use the other tooling to rough out a slightly undersized hole?
Dan,
I have tried slightly tightening the quill but I still get the side play. I'll check it again and let you know how much.
thx for the input.
Jim
 
A step drill will start the hole and guide a regular drill bit better.
 
scattermaster said:
Ok,
I'm working with cast iron hydraulic pump housings. (ductile iron maybe?)
The existing holes are 12mm diameter and 13mm deep. 180mm spacing on centers. I don't have a tolerance for that spacing but my experience tells me that I have have to be within 3 or 4 thou between the pair. So theoretically I could be .002" off center on both and still be in spec.
I want to be inside of that.
The new holes are 16mm diameter, -.000mm +.018mm. (.6299"-.6306" for a .0007" tolerance) with a 15.5mm depth at the bottom corner of the hole. (not the center)
The pins that go in the holes are 16.023mm-16.034mm. I measured 2 samples and they are right at .6312" dia. (16.0324mm)
I think I should shoot for the large end of the tolerance on my holes.
My customer is needing 4 of these per day and there is also another piece that has to be done as well. So, yeah it's a production run and I'm concerned that boring will eat up too much time.
Possibly I could get my boring head set to achieve the perfect diameter and use the other tooling to rough out a slightly undersized hole?
Dan,
I have tried slightly tightening the quill but I still get the side play. I'll check it again and let you know how much.
thx for the input.
Jim
Click to expand...

I have ran Big Devlig jig boring machines and even a SIP. .002" is about the best you can hope for with twist drills and a reamer, especially if your doing it with a drill chuck. Many jacobs have that in runout!. Using a er collet tool holder will help as will higher end carbide drills but still you will have consistency issues due to the limitations of twist drills.

The boring really needs to be done over two or three passes to true it up. If you try do it all in one pass you will have run out issues. Maybe a quick change tool system like tts can have 2 different boring heads set up so your not adjusting them?

As far as play, if doing precision work on a machine with a less than ideal quill, lock it and move the knee on the critical passes.
 
If you are using a standard jobber drill, then most likely the drill is walking when you start the hole. I use mechanics length/short drills on my mill and if I need high precision I center drill the hole first. You also have flex in the chuck system, I would use something like an ER-32 collet holder and consider a short carbide drill. I assume your Z axis is locked and you are drilling with your quill, there may be limits to the rigidity of the mill due to the longer Y axis and flex. One should see if it is the head that is moving or just the spindle. I also use a vacuum at the drill hole when drilling cast iron to reduce the chance of regrinding and enlarging the hole. I do have projects where I drill cast iron and I need to maintain a 0.001" accuracy center to center distance between holes. Standard drills/chucks does not work.
https://www.mcmaster.com/drill-bits...gth/for-use-on~iron/maximum-drilling-depth~1/
 
You must log in or register to reply here.
Back
Top