Tooling ideas

[BBprecise]

Got an aluminum 7075 part that needs a Ø1" hole 7" deep that's full radius at the bottom. +/-.005 on size and depth. My thought is to drill it to 1" (maybe a little under), then get a ballnose made up with cylindrical ground flutes (non side cutting) and finish the bottom with that. Customer is very critical when it comes to cosmetics so I need to have a consistent finish top to bottom.

 

Looking to get other ideas on finishing this hole? CAT40 mill.

 

Thanks.

[Rstewart]

Does the blend from the wall to the radius have to be perfect? 

 

I would bore the straight section about .003" over and then send a 1" ballnose in.

[taperlength]

I had a job like that and the 1" ball chattered at the bottom, so I used a .75 ball and a swept toolpath for the full radius.

[Reko]

Ingersoll make coolant through drills that can hold that diameter and I believe they do a 7 to 1... not sure though. The bottom can be blended in with a long end mill.

[BBprecise]

Stewart, the blend doesn't have to be perfect, but the closer the better. Our finishing dept. can do a little polishing easy enough, but the less they have to do the better. I may end up reaming the hole.

 

TL, I have same concerns as you sticking that ballnose out there so far.

 

Reko, Iscar has a double margin Sumocham drill that I think goes up to 8D that I was thinking about using, but haven't had a chance to do anything with this since this morning. Had some IT problems to deal with 1st.

 

Years ago we did a similar job and had an AMEC T/A insert ground with the radius and drilled it in one shot. Worked ok, but the finish wasn't great and wouldn't be good enough for this customer.

 

Just got to looking at the model and the bottom of the hole intersects another larger hole and the reach is under 2" so I think I'm gonna try drilling to size on 1st op. and then mill the radius on the 2nd op.

 

Thanks guys.

[BBprecise]

There's a note on the print "Trajectory of machined features". Any of you ever seen/know what this means? Looks like they're trying to control/dimension some 3D surfaces,but never seen it done like this before. I've done parts where the grain structure of the material has to be orientated a certain way in relation to the part, but I don't think that's what they're trying to do here.

 

Thanks.

[TERRYH]

In the past we have had our tool crib grind flat bottom drills and drill it to depth with a regular drill and then go back in with the flat bottom, if I understand what your wanting to achieve.

[Guest]

The only time I have ever seen "trajectory" was when the "engineer" meant "projected tolerance zone". It took an hour and 3 QC guys to back me up. Basically the part I was working on was .250 diameter 4x D with a projected tolerance zone of 2.5" and the tolerance was +/-.0005. It was a bear of a part.

 

HTH

[Newbeeee™]

Can you drill it, then ream it, then use a form tool.

Form tool to be a reamer style shank but ground with a ball end. Then just peck drill the bottom - very small peck depth to break swarf but not induce chatter so the tool doesn't  want to 'kick'/vibrate?

Never heard of the words "Trajectory of machined features".

If in doubt - ask!

[BBprecise]

I've dealt with projected tolerance zone on a hole before and it can definitely make it a challenge, but never seen anything like that applied to a profile. Our process engineer has been out the last couple of days, but should be in this morning so he's going to shoot of an email to the customer.

 

Newb, I was leaning towards what you're thinking until I realized I can get to the bottom from a cutout on another side of the part, so I'm gonna go in with a ballnose from there.

 

Thanks.

[Tim Johnson]

Could they mean surface profile?

 

[BBprecise]

Maybe Tim. If so , I've never seen it called out like that before in 20+ yrs. Hoping to hear from customer this morning.

[MrFish]

We used to drill a hole similar except 1 1/2" dia (actually 40mm as I'm in land of metric) that needed a "cupped" bottom and hand dressed a HSS drill with the ball on it. It actually drilled really well, held size and had good swarf flow. Was in a lathe so was effectively self centring but might be worth a try. Hardest part was grinding the centre of the drill tip.

[jlw™]

I've used 2 flute ball mills the same way. Only difference is you don't have to grind them yourself. 1in was the biggest we ran.

[BBprecise]

Thanks guys. As of right now I'm gonna try to get it from a shelf that's cut into the bottom of the hole at a right angle to it. Only issue will be the blends if hole isn't drilled straight. Finishing dept. may have to do a little hand blending, but that's what they're for.