Under cut guidance 1

[cjccmc]

I am working on a design that when finished looks like a circular plate with T shaped stiffeners (like wheel spokes) 30 degrees apart. All the T stiffeners are oriented to run thru the center of the circle plate. The top (flange) of the Tees are 3 inches above the plate. This part to be machined from 7075 Al plate 4" thick. The T flange is 1.2" wide, has a .2" web, so I need to under cut .50" from each side to end up with the T shape.

What makes it complicated is all the other features that need to be provided. It's important to remove as much material as possible for weight reduction. Can someone give me pointers about cutting tools that can hog out the material between the T flange and circular plate? I'm looking for enough info to make the design producible, so data on cutter diameters and the related shaft diameter will help me layout proper clearances between features. thanks!

 

[BillPSU]

I can't visualize what you are describing. A sketch would be in order for this.

Bill

 

[MikeHalloran]

A big T-slot cutter is the obvious tool, I'm guessing 2" diameter with a 7/8" shank will do. That may be a custom tool.

Next choice might be stacked saws on a cantilevered spindle.

In both cases, you rough out the vees with a big end mill. Plunge cutting might be fastest.

Either way, you can't cut in to the center of the circle, so you have to leave that solid, or bore a big hole there. ... or EDM that area.

Don't be surprised if the big plate warps when you remove material asymmetrically.

Consider cutting T-slots in a thinner plate, and pressing in H-sections to form your fins. They can be mitered to meet in the center with no hole and no solid mesa.





Mike Halloran
Pembroke Pines, FL, USA

 

[hendersdc]

Do you need the other side of the plate to be solid or could you hit the under cut from the other side?

Have you considered a weldment to avoid needing to core our a 4" thick plate?

Can you go with a cast grade of Al to minimise the warping Mike talks about?

Doug

 

[cjccmc]

Thanks for the inputs. Welding is not an option due to part funtion and program reqmnts. Are there any supplier catalogs showing dimensions for common cutting tools that could do this?
See attached for prelim idea of final part.

 

[MikeHalloran]

The part has a certain bizarre beauty, but it will be a nightmare to make.

I.e., your supplier will get some awards from his trade association, and you'll buy him a new Porsche.

In current form, the only way I can see to produce it is as a lost-wax casting to net shape, or damn near it.

The radii tangent to the webs at the bottom of the pockets are currently impossible; they must have the same radius as the T-slot cutter or larger.
...
Belay that; you can get in there and generate them with a really small ball end mill if you have a tilting spindle or indexing table.


Mike Halloran
Pembroke Pines, FL, USA

 

[hendersdc]

This part would be much easier to machine without the "T" portion of the stiffener ribs. Could you get away with vertical or drafted ribs without the top? They would need to be taller or thicker (and slightly heavier) to keep the same rigidity. Without knowing your application it is hard to know if the cost is worth the weight savings.

These guys Link specialize in dificult 5 axis jobs. You could contact them for more detailed suggestions/quotes.

Doug

 

[cjccmc]

"Could you get away with vertical or drafted ribs without the top? They would need to be taller or thicker (and slightly heavier) to keep the same rigidity. "

We need to stick with the current shape for reasons that are too long and boring to explain, but I see your point about equal stiffness from taller ribs.

"The radii tangent to the webs at the bottom of the pockets are currently impossible; they must have the same radius as the T-slot cutter or larger."
Yeah, that's the aspect that causes me concern. I have .90 R where the short bosses transition to the vertical wwebs in the undercut area. Does that seem adequate?

There is an existing part made years ago very similar to this one. I only have photos to go by, but it did have bosses in the undercut area where access for an end mill is blocked by the tops of those T's. Not sure who made it and how $$ it was.

 

[cjccmc]

I do know that it was machined from one thick plate, not a casting or weldment.

 

[MikeHalloran]

Well, okay, it's possible to do something off the wall, like stick a flycutter down there, lock the spindle, and basically use a CNC mill as a CNC shaper, but it's going to be slow and therefore expensive. Maybe two Porsches' worth...


Or, it might be possible to mill it with tall fins and then bend them over into angles, but most of the alloys that machine well don't bend well, and conversely.



Mike Halloran
Pembroke Pines, FL, USA

 

[ajack1]

Cjccmc if I am understanding correctly you are saying that the undercut is .5” wide and the smallest radii is .9” that is possible. You would need a special T cutter of say 1.75” dia with the centre bar less than .75”.

Looking at the length of those undercuts that is going to be one spindlely cutter and is going to sing at a nice high pitch and you will almost certainly need a few of them.

But if what I am assuming is correct and there is nothing I am missing then yes what you have is possible to machine, the cost on the other hand might make you sit up and draw breath.

 

[cjccmc]

"You would need a special T cutter of say 1.75” dia with the centre bar less than .75”.

Yes that's what I'm thinking. to get .50 undercut with 1.75 cutter, it limits the shaft dia to .62

 

[BillPSU]

Reaching down the full length of the web will be the toughest problem. The cutter will be extended out about 3" and you won't be able to have anything protrude below the cutting tool. I recommend that the shank of the cutter be made out of solid carbide to give you some rigidity. The enclosed slots where the offset hole is located you will have to make sure the cutting tool can drop inside of the openings.
Plan on using a high hook angle roughing end mill for roughing out the slots. You will have to watch the re-cutting of the chips. The best thing to do would be to have high pressure air blowing the chips out the of cut.

Distortion of the whole part may be a problem. You may have to rough machine the part and attempt some kind of a stress relieve and then finish machine. You are turning about 75% of the material into chips.

Good Luck on this part.
Bill

 

[cjccmc]

Thanks for all the inputs. It will be interesting to see what kind of response we get when this goes out for bid.

 

[ajack1]

If you are putting it out to quotation at shops that are used to working on complicated aerospace or F1 or high end motor sport parts you should not have a problem, other than the price. If you just send it down the road to the nearest guy with a couple of CNC mills I think you will need a large chunk of good luck.