Concentricity of gun drilling

[badger2011]

I am machining a 16" cannulated shaft (.75 OD). There are 2 IDs which are gundrilled separate from each side and meet in the middle. I am having issues with the holes lining up, concentrically, where they meet in the middle. I am allowed a .006" tolerance on concentricity. Our machines are capable of making good parts, but about half appear to be out of tolerance (visual check looking down cannulation, at the shoulder).

Is there a method to measure this concentricity? I know I can make gages, but I don't have alot of time.


Thanks in advance for any guidance you can offer

 

[Belanger]

Just to verify -- is it the GD&T symbol for concentricity (one small circle inside another)? And does the drawing reference ASME Y14.5?

I ask because the word concentric in regular conversation is a little different than the GD&T definition, in terms of measurement.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

http://www.gdtseminars.com

 

[badger2011]

The customer actually forgot to put it on the print, part of the reason we had this issue in the first place (ugh)

They do have a .006 run-out tolerance from the smaller ID to the larger ID (the larger ID is the datum referenced)


Thanks for asking for clarification; in a nut shell, I need the two ID's to line up with in .006" when they meet in the middle.

 

[powerhound]

So if the step in the middle were able to be measured, it could be no more than a .006 step...is that correct?

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[badger2011]

See attached. The holes need to match up.

 

[Belanger]

From that latest picture, I think a runout measurement would register as .012.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

http://www.gdtseminars.com

 

[dingy2]

The total runout measurement would be .012 as Belanger stated. I am going to assume that that OD is the datum??? If that is so, then trying to get a dial indicator with contact into a small hole that is 16 inches long is pretty tough. I don't know how you would do that.

Now, if you just want to make sure that both holes on each end to match in the center with a difference of no more than .006, then maybe a straightness tolerance of .006 beyond the MMC and make both IDs at the smallest allowable size. Now you can make a checking fixture which should be straight pin with a size that is .006" smaller than the smallest allowable size. Push the checking pin in one end of the hole and, hopefully, through to the other end. If it goes, then the step is less than .006. If it doesn't go all the way, then the step is too large or the hole is not straight.

Dave D.

http://www.qmsi.ca

 

[powerhound]

I agree with the others, so if the runout tolerance on the print is .006, then your drawing shows an incorrect representation of it. As JP stated, you are showing .012 runout, not .006. For a runout spec of .006, the step between the bores can be no more than .003. This is exactly the reason I asked the question earlier in the thread.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MechNorth]

Curious why nobody's recommending a position tolerance for each bore hole wrt a datum established by the OD? A tolerance of DIA 0.012 would achieve a limited radial mismatch of 0.006 at the interface, would it not? Suggest RFS. Find the AME of each hole to establish the feature axis, and away you go.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[Medmaker]

If I'm understanding correctly, there are two different sized holes gun drilled from opposite sides. The larger one is a datum and the smaller one references it for runout, position, etc. I'm assuming this part mates with something that also has a large and small diamter that mates inside. From what has been commented so far, it will be difficult to measure something that deep (assuming it is at least 8") without a gage. I think a simple functional gage would work best. A shaft with diameter of the big hole at MMC and a short stepped diameter at the virtual condition of the smaller hole. Might not be theoretically correct, but from a functional standpoint might be acceptable.

My other comment would be perhaps a change in process. Depending on the difference in diameters, could you gun drill the small hole all the way through, turn the O.D. on centers to true up the outside, then drill/ream the larger O.D. hole with standard tooling. The larger I.D. tooling should follow the gun drilled hole and you'll avoid a lot of the mismatch.

 

[dingy2]

Medmaker:

As I understand the question, there is nothing about 2 different size holes drilled from each end but the process had each hole (probably the same size) drilled at opposite ends. Apparently, there is a mismatch in the centre. That is how I read it anyway. I don't believe there is anything in the original statement relating to the 0.750 OD except to state that it is 16 inches. Concentricity and positional require datums and it seems that we don't have any. Badger2011, we need more clarification. There are a lot of knowledgeable people here who can help. Are you only looking at the mismatch on the ID? Are you interested in the relationship of the ID to the OD (concentricity, circular or total runout, positional)? Clarification please.

Dave D.

http://www.qmsi.ca

 

[badger2011]

"there are two different sized holes gun drilled from opposite sides. The larger one is a datum and the smaller one references it for runout, position, etc. I'm assuming this part mates with something that also has a large and small diamter that mates inside. From what has been commented so far, it will be difficult to measure something that deep (assuming it is at least 8") without a gage."

^^^This is all true^^^

Clarification: it is a .006 total run-out, not .012. My picture was incorrect, my apologies.

The 2 sizes on the ID, which meet in the middle, are Ø.375 and Ø.438.

My machinist wants to order a longer gun drill to drill the Ø.375 hole 9" deep, then follow it with the larger Ø.438 gun drill. This will ensure the holes are concentric with one another, BUT there may be a mismatch when we enter the opposite side and gun drill back towards the stepped hole with the Ø.375 gun drill.

Also, I've machined a functional gauge to check this concentricity run-out of .006 so we can check the parts coming off the machine.

My remaining question for all you, and thank you again for you help already, is: Is there any machining techniques that might further help us make good parts? We are running these on swiss machines.


Thank you!

 

[Medmaker]

My only suggestion would be to get somebody to make you gun drilled blanks with the smaller diameter all the way through. Something tells me gun drilling on a swiss is limiting you. 16" inches should be achievable on a dedicated gun drill. The runout should definitely be achievable especially at that diameter.

 

[powerhound]

My only suggestion would be to make sure that if your gun drill point is 118 degrees, be sure to use a 120 degree spot drill and be sure to dwell for a second or so before retracting. I know that sound elementary. I'm just putting it out there.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MikeHalloran]

Speaking of drill points, let's back up a bit and verify that we're all talking about the same thing.

Twist drills (the kind with two flutes) are available in common sizes in lengths up to 12". They are called 'aircraft drills'. They are not gundrills, and using them is not gundrilling, it's just deep drilling.

Gundrill bits have only one flute, so they don't have a point angle in the usual sense. They are guided by the diameter of the hole already drilled, which also means that the hole must be started with a twist drill before the gundrill is inserted.

So, we have to ask for clarification of the OP: Are you just drilling a deep hole with extra long twist drills, or are you actually using gundrills?


Mike Halloran
Pembroke Pines, FL, USA