How should I tackle this part?

turbotadd · Jun 22, 2017

Wondering how I should go about making this part, Qty. 3. I have 1.5 x 13.13 x 13.13 6061 plates for material. Would it be best to drill all the holes and pocket the reliefs, then try to use the thru holes to hold it down to a subplate? I would add additional holes on the inside and outside. Or bolt up through the subplate to the 3 tapped holes? My concern with doing that is that there is too big of a span between bolts, will get chatter when I do the finish pass around. Thinking 5/8" rougher and 1/2" 3fl carbide finisher.
Machine is 40 taper VMC w/ 20"X 20"Y 16"Z.
There must be a better way...

Ox · Jun 22, 2017

I would profile either the inside or outside, and then (w/o moving it) clamp that down to some sort of bolster plate, and run the rest.

I guess the easiest would be to clamp the outside down, blow out the inside, and then clamp that down, remove outside clamps and finish.

Just have some holes already tapped inside the bore - in the bolster plate ahead of time and you're all set.

--------------------------

Think Snow Eh!
Ox

guest · Jun 22, 2017

I would probably rough the whole thing out +.100 first, leaving 4 tooling tabs around the periphery. Then let the part unspring, and bolt it back down using the tool tabs so the part is in a relaxed state. Put in the hole pattern and profile to finish, machining most of the tool tabs away. Unbolt from the plate and cut the remainder of the tool tabs off on the band saw and blend.

Cautious because I don't know how much that thing is going to spring when all the material is removed from the inside, the B.C. is a 3 place tolerance which could easily go out if you put in the holes while it's still a plate.

706jim · Jun 22, 2017

Drill the 6 0.33 holes through and drill and tap the 5/16 holes with the rectangular material held by clamps or in a vise.
Run an end mill over the inside and outside profile about 0.010 deep to mark the part. Maybe cut those 0.35 reliefs at the same time.
Bandsaw the bulk of the material away leaving maybe 1/8-1/4 stock all around. With a sharp blade, this will save you a LOT of time milling.
Now bolt it down to a sacrificial fixture plate with as many of the fasteners as possible then finish profile the parts.

Or some variation on this general idea. Hope this helps.

Finegrain · Jun 22, 2017

Since you already have 1.5" stock for a 1.5" part ...

1. Bandsaw within .1" or whatever you are comfortable with
2. Material can now go sproing or whatever the tech term is
3. Clamp it down and drill & tap the holes and mill the slots
4. Make a fixture plate with the 9 holes -- for the holes corresponding to the .33" holes in the part, first 1/4" drilled to .33", then another 1/2" deep tapped 1/4" x 20. Other 3 holes just drilled and tapped 1/4" x 20.
5. Locate the part on the fixture plate with dowel pins through a couple of the .33" holes
6. Bolt it down through the other holes, remove dowel pins, replace with bolts
7. Profile and chamfer

Regards.

Mike

deadlykitten · Jun 22, 2017

hy

... cut at oxy / waterjet / etc
... grind 2 faces
... put it above the table at 5mm on little prisms
... clamp it from the outside and machine the inside
... clamp it from the inside and machine the outside

Mtndew · Jun 22, 2017

Clamp it down
Do the holes, rough the cutout
Release
Bolt down with the holes
cut the shape
profit

Chatter shouldn't be an issue.

doug925 · Jun 22, 2017

I think you are stuck with a 2 opp part, regardless of using a fixture plate or not.
I'd probably go with (post #) 3 or 5

If I had to make 3 of them, I would start with 2" plate, clamped in the corners.
Face to top, drill, drill/tap the holes, mill the slots.
Remove the bulk of the material down 1.75" or so, leaving only the corners and part.
Use a keyway cutter to cut the part from the material below.

This could be done in 1 operation.

Just my $.02,

Doug.

plastikdreams · Jun 22, 2017

That's gonna spring like a slinky! I too would rough the shape first, let it spring to shape, and then do all the finish work. In actuality I would use the holes to hold it down to a plate and then run an endmill around the periphery in a constant ramp.

I hope you charged well lol.

countryboy1966 · Jun 22, 2017

How often do you all quote a job you don't even know how to make seeking advice on the internet and hope you make money?

I'm not attempting to rub the OP the wrong way, but just curious is all from a non-contract machine shop perspective. :cheers:

I realize I am making some assuptions. lol.

plastikdreams · Jun 22, 2017

countryboy1966 said:
How often do you all quote a job you don't even know how to make seeking advice on the internet and hope you make money?

I'm not attempting to rub the OP the wrong way, but just curious is all from a non-contract machine shop perspective.

I realize I am making some assuptions. lol.

Woah woah woah...woah, that's not how it's done?

Mind...blown!

thesidetalker · Jun 22, 2017

countryboy1966 said:
How often do you all quote a job you don't even know how to make seeking advice on the internet and hope you make money?

I'm not attempting to rub the OP the wrong way, but just curious is all from a non-contract machine shop perspective.

I realize I am making some assuptions. lol.

Poster isn't always the person to quote it, so I don't think you can necessarily place blame there so quickly.

Where I work the boss, which doesn't know much about machining in general, does the quoting and mostly makes use of the dart board technique. Some jobs are losers, some are real winners. Guess it works? Been here a while.

Limy Sami · Jun 22, 2017

Yup, whatever you do that part is going to be full of stresses, so cut it well oversize and leave it to squirm like the village virgin on a bar stool then finish machine.

FWIW I like the clamping taps idea, because if it moves too much your circle of holes will be all wrong, so leave those until the 2nd op.

FWIW 2 When I do jobs that are going to move, I rough out and leave them for at least 12 hours on top of the boiler were it's about140 - 150 F which speeds up the process no end.

dksoba · Jun 22, 2017

thesidetalker said:
Poster isn't always the person to quote it, so I don't think you can necessarily place blame there so quickly.

Where I work the boss, which doesn't know much about machining in general, does the quoting and mostly makes use of the dart board technique. Some jobs are losers, some are real winners. Guess it works? Been here a while.

I put a bit more work into my quotes. Some jobs are losers, some are real winners. I think I'm going to start taking the dartboard approach.

Ox · Jun 22, 2017

Limy Sami said:
Yup, whatever you do that part is going to be full of stresses, so cut it well oversize and leave it to squirm like the village virgin on a bar stool then finish machine.

FWIW I like the clamping taps idea, because if it moves too much your circle of holes will be all wrong, so leave those until the 2nd op.

FWIW 2 When I do jobs that are going to move, I rough out and leave them for at least 12 hours on top of the boiler were it's about140 - 150 F which speeds up the process no end.

Or just start with cast tooling plate....
You're not saving any $ usually by going with the moving material in apps like this.

----------------------

Think Snow Eh!
Ox

Misterwidget · Jun 23, 2017

I would clamp it to 1 2 3 blocks right on the table. Finish all holes. Rough an finish inside, using a Niagara 3/4 Elite ( 3/4 dia,2 1/4 LOC ) , move clamps, and blocks, 1 at a time, so as to not lose location, to the inside Finish the outside.

Misterwidget · Jun 23, 2017

6150 is fairly stable especially at 1.5 thick,I don't thin it will move mutch. Run the elite at 3500 rpm,45 inpm and step it down .400 at a time.

Finegrain · Jun 23, 2017

Ox said:
Or just start with cast tooling plate....
You're not saving any $ usually by going with the moving material in apps like this.

If the spec allows -- when drawing says "6061" they might be peeved if you deliver MIC-6 or similar.

Regards.

Mike

Limy Sami · Jun 23, 2017

Misterwidget said:
I would clamp it to 1 2 3 blocks right on the table. Finish all holes. Rough an finish inside, using a Niagara 3/4 Elite ( 3/4 dia,2 1/4 LOC ) , move clamps, and blocks, 1 at a time, so as to not lose location, to the inside Finish the outside.

And watch it move with stress relief, ....hole positions and everything will be out, I doubt if it will even stay circular.

LKeithR · Jun 23, 2017

Limy Sami said:
...leave it to squirm like the village virgin on a bar stool...

Here I go derailing the thread a bit but I really do think Limy should start a thread of daily quotes--he seems to have enough zingers
like this that he could post one a day forever... :eek:

And I do agree that the part is going to move if it isn't allowed to relax after most of the material is removed. However, one thing that
hasn't been considered is how the part mates to whatever it is attached to. If there is a dimensionally accurate groove, shoulder or
other feature on the mating piece that locates this part then a little spring may not matter so long as the part is pulled back into shape.
It depends to a degree on what accuracy is required of the fully assembled unit...

How should I tackle this part?

Aluminum

Diamond

guest

Guest

Titanium

Diamond

Banned

Diamond

Titanium

Diamond

Hot Rolled

Diamond

Stainless

Diamond

Hot Rolled

Diamond

Plastic

Plastic

Diamond

Diamond

Stainless

Similar threads