make sure your dowel holes are on location!

[JBrentMac]

This is kind of embarrassing, but hopefully it will help others
I just did a job where each part had three .188 holes +.001 -.000. Slip fit. no problem. But, location had to be within .001.
I have no idea ho the ones I 1) spotted, 2) drilled, and 3) reamed ended up off location. i mean the spot drill i used was a .375 dia. going into a circle milled hole (cirular interpolated on a CNC mill to hold both diameter and depth within .0005) of .385. apparently that was enough wiggle room to **** me.
Could it have been something wrong with my spot drill?
Any way, to avoid this problem in the future, use a drill that is at least .03 smaller than your reamed hole should be (instead of .01-.015).
'But doesn't that leave too much stock to load up your reamer makining it cut over size?'
Hold on- then you take an undersized (reground) end mill...:thinking:
For instance:
Print calls for a .25 PF(press fit for dowel)
Use a no. 7 drill (the tap drill for a 1/4-20), a 1/4 end mill that has be reground (cuz it needed sharpened) to .240. Then ream. that way if your drill leads off, or you just might have accidently spotted it off a couple thou, the end mill will bore you a straight hole on location.
'Wait! What about metric?"
OK! Print calls for 5h7. you don't need a regrind! 5mm=.1969. use a 3/16(.1875) end mill.
I know there will be instaces where this formaula won't yeild the most compatible pairings, but that didn't seem to bother my supervisor while he was simultaneously teaching me this trick and chewing my @$$ out.:*****slap2:

 

[dickr]

You mentioned a "SPOT DRILL". Is that a shortened drill or a center drill. A spot drill can easily go off center. I always use a center drill (USA made) not resharpened. When you start getting that close in your work there are many things that can go wrong. Turn the machine on, locked the table in that order. They make V pointed mills now that would help. You may have even sneezed at the wrong time. It sounds like you learned a lot on that one so at least you're that much more ahead. Don't beat yourself up, just sharing that experience will help others like you said.
dickr

 

[frankie]

I a gree with dickr, I have tried spotting drills a few times the results were less than expected so I use only center drills to locate holes.

frankie

 

[Walt]

This is kind of embarrassing, but hopefully it will help others
I just did a job where each part had three .188 holes +.001 -.000. Slip fit. no problem. But, location had to be within .001.
I have no idea ho the ones I 1) spotted, 2) drilled, and 3) reamed ended up off location. i mean the spot drill i used was a .375 dia. going into a circle milled hole (cirular interpolated on a CNC mill to hold both diameter and depth within .0005) of .385. apparently that was enough wiggle room to **** me.
Could it have been something wrong with my spot drill?
Any way, to avoid this problem in the future, use a drill that is at least .03 smaller than your reamed hole should be (instead of .01-.015).
'But doesn't that leave too much stock to load up your reamer makining it cut over size?'
Hold on- then you take an undersized (reground) end mill...:thinking:
For instance:
Print calls for a .25 PF(press fit for dowel)
Use a no. 7 drill (the tap drill for a 1/4-20), a 1/4 end mill that has be reground (cuz it needed sharpened) to .240. Then ream. that way if your drill leads off, or you just might have accidently spotted it off a couple thou, the end mill will bore you a straight hole on location.
'Wait! What about metric?"
OK! Print calls for 5h7. you don't need a regrind! 5mm=.1969. use a 3/16(.1875) end mill.
I know there will be instaces where this formaula won't yeild the most compatible pairings, but that didn't seem to bother my supervisor while he was simultaneously teaching me this trick and chewing my @$$ out.:*****slap2:

Sorry to hear you had a rough day!

Am I understanding you correctly? Your boss wants you to bore the drilled hole with an undersize end mill, then ream to size?

If the spot wasn't placed correctly though, the end mill could be bored off by exactly the same amount, gaining nothing. Sounds like your boss thinks the deep drill wandered off of a correctly drilled spot. Someone with more experience, please comment.

My understanding is spot drills are as rigid as center drills, but less likely to break off in the hole.

Walt

 

[Tom Griffin]

If you want location to be within .001" you need to be boring not drilling and reaming. It's nearly impossible to hold a location that close with a drill. Moore Precision Tools made a business based on that fact with their jig boring machines.

Tom

 

[kd4gij]

.

My understanding is spot drills are as rigid as center drills, but less likely to break off in the hole.

Walt

A spot drill doesn't drill a pilot hole so the drill can still wander. A center drill leaves a pilot fo the drill to fallow.

 

[Walt]

A spot drill doesn't drill a pilot hole so the drill can still wander. A center drill leaves a pilot fo the drill to fallow.

I admit that I can't drill a hole and end up with a location accurate to within 0.001" using a spotting drill followed by an ordinary twist drill. Are you saying that using a center drill will guarantee that a regular drill won't wander? If this works for you, that's wonderful. My experience is that holding a location to within 0.001" with a twist drill isn't going to happen regardless of how accurately the hole was started.

Walt

 

[Bill C.]

This is kind of embarrassing, but hopefully it will help others
I just did a job where each part had three .188 holes +.001 -.000. Slip fit. no problem. But, location had to be within .001.
I have no idea ho the ones I 1) spotted, 2) drilled, and 3) reamed ended up off location. i mean the spot drill i used was a .375 dia. going into a circle milled hole (cirular interpolated on a CNC mill to hold both diameter and depth within .0005) of .385. apparently that was enough wiggle room to **** me.
Could it have been something wrong with my spot drill?
Any way, to avoid this problem in the future, use a drill that is at least .03 smaller than your reamed hole should be (instead of .01-.015).
'But doesn't that leave too much stock to load up your reamer makining it cut over size?'
Hold on- then you take an undersized (reground) end mill...:thinking:
For instance:
Print calls for a .25 PF(press fit for dowel)
Use a no. 7 drill (the tap drill for a 1/4-20), a 1/4 end mill that has be reground (cuz it needed sharpened) to .240. Then ream. that way if your drill leads off, or you just might have accidently spotted it off a couple thou, the end mill will bore you a straight hole on location.
'Wait! What about metric?"
OK! Print calls for 5h7. you don't need a regrind! 5mm=.1969. use a 3/16(.1875) end mill.
I know there will be instaces where this formaula won't yeild the most compatible pairings, but that didn't seem to bother my supervisor while he was simultaneously teaching me this trick and chewing my @$$ out.:*****slap2:

I would use a Number 2 center drill to hold the location. I would also skip the .240 end mill.

Good luck

 

[Skip]

Many times in my toolmaking years I was called on to do exactly what you tried. I would first spot the place to put the first hole. Second I would center drill, drill and ream the hole for a slight press fit, (I would go back and ream for the slip fit after the next hole was finished.) Third I would put a dowel into the press fit hole and then indicate the pin true to the quill. Then I would step off to drill and ream the next holes. This sounds like it takes a lot of time and it does, but remember, the tolerance was put there for a reason. You may or may not be making the mating part or where the part you are making may be going into the next county or state. Precision does not come cheap.

Skip
Retired and loving it.

 

[JBrentMac]

You mentioned a "SPOT DRILL". Is that a shortened drill or a center drill. A spot drill can easily go off center. I always use a center drill (USA made) not resharpened. When you start getting that close in your work there are many things that can go wrong. Turn the machine on, locked the table in that order. They make V pointed mills now that would help. You may have even sneezed at the wrong time. It sounds like you learned a lot on that one so at least you're that much more ahead. Don't beat yourself up, just sharing that experience will help others like you said.
dickr

By spot drill i mean something like a ctr drill but without the smaller dia lead on it. suposedly they are just as effective. when i get to work on monday i'll have to look at it.
maybe the tip was wore out...
anyway, thanks for all your input you guys!