1.3" hole at 45 degrees through 1/4" stainless sheet

[kb0thn]

Hi Guys,

I have a part that will be going into a product we make. Basically it's a 1.34" diameter hole at a 45 degree angle through 1/4" stainless. I seldom do angled entry holes and I am looking for suggestions on a machining strategy for the angled hole.



I can easily have the profile and small holes laser cut on a 2-axis laser. And could laser cut out none or most of the angled hole normal to the flat face. Machine to do the angled hole would be modern Mazak VMC with CAT40 spindle. I was thinking I could do soft jaws with angled slots to allow two of these parts in a single vise. We have 300 of these to do and we'll have probably smaller quantities to do every year forever.

My default thought would be just a use a big solid carbide end mill and helical interpolate. Probably have the laser remove as much material as possible. I use insert drills with great success, but I am not sure how well they would do on the angled surface. I'd like to have relatively burr free faces so we can immediate weld without needing substantial deburring.

Any other, hopefully better, suggestions?

I did put a few RFQ's out to 5-axis laser and waterjet job shops. But they seem relatively few and far between. What I have found seem like they want to make this a $50 part. If that's the case, I'd rather get a $7 2-axis burnout and put a $7 hole in it in-house.

Thanks!

 

[Milland]

I think the vise with slotted mild steel jaws would work, unless the steel could contaminate post-machining welding. I wouldn't use Al for the jaws given the narrow grip faces.

Look into a 1/2" or 5/8" necked short flute cutter, laser most of the hole out, then use an angled X-Y-Z path to semi-finish then finish the hole. That should give you minimal cut time, and by keeping the endmill engaged with the part you lower the stress of entry/exit on it. There's 4-6 flute versions of extended length EM's appropriate for stainless that should last quite a while with the right S/F.

 

[art.h]

Hi Guys,

I have a part that will be going into a product we make. Basically it's a 1.34" diameter hole at a 45 degree angle through 1/4" stainless. I seldom do angled entry holes and I am looking for suggestions on a machining strategy for the angled hole.

View attachment 382570

I can easily have the profile and small holes laser cut on a 2-axis laser. And could laser cut out none or most of the angled hole normal to the flat face. Machine to do the angled hole would be modern Mazak VMC with CAT40 spindle. I was thinking I could do soft jaws with angled slots to allow two of these parts in a single vise. We have 300 of these to do and we'll have probably smaller quantities to do every year forever.

My default thought would be just a use a big solid carbide end mill and helical interpolate. Probably have the laser remove as much material as possible. I use insert drills with great success, but I am not sure how well they would do on the angled surface. I'd like to have relatively burr free faces so we can immediate weld without needing substantial deburring.

Any other, hopefully better, suggestions?

I did put a few RFQ's out to 5-axis laser and waterjet job shops. But they seem relatively few and far between. What I have found seem like they want to make this a $50 part. If that's the case, I'd rather get a $7 2-axis burnout and put a $7 hole in it in-house.

Thanks!

Hi Guys,

I have a part that will be going into a product we make. Basically it's a 1.34" diameter hole at a 45 degree angle through 1/4" stainless. I seldom do angled entry holes and I am looking for suggestions on a machining strategy for the angled hole.

View attachment 382570

I can easily have the profile and small holes laser cut on a 2-axis laser. And could laser cut out none or most of the angled hole normal to the flat face. Machine to do the angled hole would be modern Mazak VMC with CAT40 spindle. I was thinking I could do soft jaws with angled slots to allow two of these parts in a single vise. We have 300 of these to do and we'll have probably smaller quantities to do every year forever.

My default thought would be just a use a big solid carbide end mill and helical interpolate. Probably have the laser remove as much material as possible. I use insert drills with great success, but I am not sure how well they would do on the angled surface. I'd like to have relatively burr free faces so we can immediate weld without needing substantial deburring.

Any other, hopefully better, suggestions?

I did put a few RFQ's out to 5-axis laser and waterjet job shops. But they seem relatively few and far between. What I have found seem like they want to make this a $50 part. If that's the case, I'd rather get a $7 2-axis burnout and put a $7 hole in it in-house.

Thanks!

 

[art.h]

Angle slotted jaws in vice and drill with an 1.250 annular cutter with a knock out to kick slug and a helical to size, same cutter.

 

[DDoug]

Doo it with the 2 axis laser and be done with it.
the resulting chamfer is for welding....

 

[kb0thn]

Doo it with the 2 axis laser and be done with it.
the resulting chamfer is for welding....

I did 120 of them that way earlier this year. It was kind of a disaster. There is a pipe that goes through this flange and mates with stuff on both sides. The gap to fill is non-trivial and there ends up being a lot of heat that goes into the weldment and warps the flange. And even with a decent fixture, the weldor was making all kind of off-axis creations. It was a complete mess.

With a really tight fit-up we will be able to laser weld these with very little heat going into it. And hopefully the pipe will stay much closer to where it needs to me.

 

[EPAIII]

Fixture it in your mill at 45° and use a 1.250", carbide tooth, shell cutter to take out most of it. Then a carbide end mill for the remainder. Hopefully you have CNC.

 

[kb0thn]

Angle slotted jaws in vice and drill with an 1.250 annular cutter with a knock out to kick slug and a helical to size, same cutter.

I have been considering an annular cutter. If I was doing it in an open mill or drill press, that would be my goto method. They are pretty cheap and stout. My experience using them in the VMC is that the slug gets stuck and makes a mess. But I think I could get the laser preparatory hole sized such that there wouldn't be a slug.

Are you suggesting helical interpolating with the annular cutter? I had never considered that.

 

[EPAIII]

Or wire EDM, but that is going to be slow.

 

[mhajicek]

Laser it close, since you'll be lasering other features anyway. Make a fixture to stack a few of them at the requisite angle, and give it a pass or two with an endmill, unless you want to do corner breaks, in which case only do one at a time.

 

[memphisjed]

Laser out leaving a smidgen for a cnc knee mill doing the nod to finish. No plunge or crooked hole to drill.

Edit/add: a two axis plasma with the torch jacked to 45 degrees also works. I have done both methods, depends on hole quality which you choose.

 

[Garwood]

I would not use the annular cutter. It will jamb. And you'd be using a custom or a 1.375" tool.

I'd be in the 1/2" endmill in the VMC for 300 parts. I'd use a cheap 4 flute rougher and a good 5 flute finisher. The laser edge will destroy your rougher quickly. Try to conventional mill it.

If you use a bigger indexable tool it's going to chatter like crazy. You'll have too much engagement and it's just 1/4" plate.

I would also be prepared to build a fixture that clamps it down against a solid surface. I make a shitload of parts from mild steel that are close tolerance holes milled through steel plates. It's very easy to potato chip a plate like that holding the sides in a vise. I had a new guy make a couple thousand junk parts that way one day.

These would be ideal work for an HMC. Hell if you have a 4th it could be a worker as well.

 

[kb0thn]

These would be ideal work for an HMC. Hell if you have a 4th it could be a worker as well.

I do have a 4th in the machine. What would your approach be with it?

Thanks

 

[Garwood]

I do have a 4th in the machine. What would your approach be with it?

Thanks

If your 4th is setup or easy to setup and you have a process to quickly make up a trunnion for it that would be an way to make a fixture for these- Mill the fixture at B0. then rotate it to 45 and leave it parked with the brake on.

If the 4th doesn't live on the table or you don't have a modular trunnion kind of fixture sorted out already then it's probably best to just make a solid fixture to bolt on the table.

This would be if you don't go for vises.

 

[EPAIII]

Seems to me the diameter is the bitch. Possibly use a 1.25" annular cutter for most of it. But you are going to need a deep one to hold the slug at 45°.

And then, how about a boring head to get the final diameter. You can dial it in as you wish and just one pass. No CNC.

 

[EPAIII]

Sorry, double post.

 

[Overland]

As Memphis said, why not a 2 axis laser with head set at 45 degrees ?
Bob

 

[implmex]

Hi kb0thn:
My vote goes with Milland's strategy he outlines in post #2.
Your biggest problem is going to be the stickout of the cutter to reach through the part on the low side without crashing the collet into the edge of the flange.
Maybe a longish shrink fit holder will help you.
If you can set up the toolpath to walk the cutter down and up on the angle, it becomes a simple side milling cut and you can use a smallish, comparatively cheap endmill so long as you can stick it out far enough to reach through the part on the low side.
I love 5/16" diameter 4 flute cutters for stuff like this...thick enough to be stiff enough to push a bit, and small enough to stay below the price jump we usually see at 3/8" diameter.
You're going to trash some cutters so cheap is important if you have 300 of these to make.

It will likely be the fastest way you can make the hole without a 5 axis laser.

Make your "soft" jaws out of heavy 4140 plates and make them roof shaped so the collet can't crash into them either.
Put ledges on both ends and make them blind on the low side or put in stop pins so you can lay two parts in at a time without them sliding out of the jaws before you get a chance to clamp them.

Mill them two at a time (obviously)...one on each side of the "roof".
Avoid slotting the jaws...just make ledges like you would if the parts were laying down flat...the slots will be a PITA unless the stainless plate is very consistent in thickness and you don't mind the time it takes to slide a plate in between two slots and then get it back out again when it's all nasty with chips and burs and razor sharp edges.
If you make the slots tight, it becomes a pain, if you make them loose, there's no point, so I vote to just eliminate them from your fixture design.
Gravity will hold the plates onto the ledges just fine.

If you try to Rotabroach or hole saw these the holes will pull to the the low side and the cutter will be trashed pretty quickly in 304 or 316 stainless.
It will be worse when you core out the inside with a laser cutter first if the cutter relies on a pilot like many hole saws do.
Besides, a carbide tipped hole saw of any kind will cost a fortune in a custom size...small carbide endmills are cheap and who still wants to try to mill 304 or 316 stainless with HSS in 2022?

Milland's proposed "dipping and rising" toolpath will mean you can make a hole finished with a single contouring pass...no need to helical interpolate.
It'll be fast and accurate and easy to control the size you end up with.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[kb0thn]

Thanks Marcus and all others that responded. I've got plenty to chew on now.

Thanks,

-Jim

 

[kb0thn]

Just following up on this:
I made soft jaws at a 45 degree and used a 1/2" carbide end mill to do an XYZ interpolated hole. Absolutely perfect beautiful hole in just a few minutes.
That is as cut. No burr to speak of.

Nice tight assembly!