Thread: Any ideas for this part

I average making 1 of these parts a month. Material is 304SS and it has 4 tee slots that stop blind toward the center. I think I keep getting them because no one else wants to attempt them. I've done testing with different cutters on sample material and have settled on a cobalt rougher from F&D. I had two different factory guys come in with inserted cutters and one said no way and the other bought me a new tool holder when all was said and done. There are a few issues with it. One is the hunk of material at the blind end of the slots that I've worked out with the customer allowing me to make my pre slot go to the end, and another is that it is not a standard size and you have to make multiple passes. The tools I am using are around 200.00 each and I figure in one per two plates. Getting a cutter the right size made costs much more and I'm not sure it could take the cut. Right now what has worked is 4 passes. Two down the middle and two climb cuts taking it to size, varying depth. The rubbing action coming out of the slot I believe is the main thing wearing the cutters out. Ive tried using only 2 climb passes and it is just too much for it. I've tried two different people, one the factory, for resharpening the cutters and when resharpened they only last one slot. The only speed and feed combo that has worked is 255 rpm and 2ipm. Very slow, but try getting the tool out of that holder with it buried in the part. It's not fun. Not had to do it because of failure, but because of a power outage. The material is very expensive and supplied by the customer. Any ideas to make this less stressful. My butt hole draws up every time I hit the cycle start button on this one.

Well lots of info but..
What are dimentions of T-slot and the cutter you are using?

The only idea I have is to beg for a change of material . I guess they're welding the finished part though?

Regards.

Mike

Cutter is 1.25 x .480 standard 5/8 tee cutter. The slot is 1.540 x .607 with the opening .915. Sorry I didn't spell that out.

I do make some of these from a36 and they're not as bad. Still a pucker factor though

If you could get the slot to go through this would be simple on a shaper

Cant go through. There is a series of oring grooves in the middle as well as a 4" hole all the way through the center not shown. Slots are for clamping a part sealed against the orings for testing. They wont use a standard tee nut, only an oversized one from Jergens.

have you tried Tialn coated tools in that? I've run them dry in 304 with no problems.

you could try and have the outside parts of the t gun drilled first removing most of the material and then finishing with the cutter you have. i would assume since your running so slowly that chips are a major issue. or you could send it out for edm. probably too expensive, but worth a shot.

Are you making a slot first that goes just past(.020") the finished depth you need? We always do that to take out as much material as possible before using a T slot cutter. Can you get a standard roughing T slot cutter to take out most of the material? Other than that, lots of coolant to flush the chips out of the slot so you don't re cut them. Hope you have a rigid machine and patience. Not too many shortcuts with 304 and T slots. Variable flute cutters for the slot will make a world of difference, but I've never seen them for T slot cutters. I have not seen insert T slot cutters that small.

What about making it modularly? You could dowel and bolt a cap instead of milling a t-slot?

I just googled this up have no idea, just a 3 second check on geometry seems like the top two could work..

T-Slot Cutters

But curious about the inserted cutter and why thats no good...seems like the more you could undercut/takeout with inserted tools (with changeable edges) the less you'd have to move with the cobalt finisher...

Rjt. I am making the slot .02 deeper. I was able to talk the customer into that in the beginning.

Proturn. I did talk to them about this and they gave me a lecture on sealing pressures and dispelled it.

Matt. The insert cutter I tried worked in my initial test with a thru slot although it sounded terrible. Where it failed was when it had to come back out at the blind spot. I think the direction shift allowed the deflection to settle and the inserts broke. When they go the body goes and the part goes, and in my case the tool holder too. I think anything carbide will do this in that transition.


Chip evacuation is definitely a major issue. When I tried only using two passes climb milling, other than vibration, the extra chips had nowhere to go in the turnaround. The machine setup is as rigid as I can make it. I tried milling chucks and a hydraulic holder, but the best has been the stub EM holder. I actually get two plates out of the cutter instead of one using this holder over the others. I do have to put the part up on parallels to put the thru hole in it but I leave that for another op after the tee slots.

Looks to me like you need a cutter less than 1.2275 diameter. That way you could climb cut in, arc around the blind end and climb cut out. I don't find anything between 1.25 and 1.0 other than an Iscar MM GRIT 28K ..... at 1.091 diameter, but it only undercuts .236 and you need .3125.

Here is a picture of the part before I put the 4" hole through the center to clear up why the slot has to be blind. Alphoso, you bring up a good point about a cutter not hitting both sides as it goes around. I just worry that even If I do spend the money to get a tool made the right size that it may not work. In that turnaround the chips have nowhere to go. Two different sized tools like you mention may work. One would be smaller for roughing and the other on size for finishing. Having the smaller tool roughing might give it a chance to get some chips out of there I dont know. I think its alot of expense to try, but I might if the volume picks up.

It might be a case of less is more. The tool is too wide to cut at a proper feedrate in that material. I'd suggest grinding it to about half of its normal thickness, relieve the end that you ground flat and then feed it quite a bit more aggressively, while keeping the rpm low and the coolant on full.

Originally Posted by alphonso

Looks to me like you need a cutter less than 1.2275 diameter. That way you could climb cut in, arc around the blind end and climb cut out. I don't find anything between 1.25 and 1.0 other than an Iscar MM GRIT 28K ..... at 1.091 diameter, but it only undercuts .236 and you need .3125.

Sounds like a plan.
This way you don't need to cut air.

Aren't there any TSlots with the same 1.25 Dia and 3/4 Shank?.
This and also having shorter stickout would make alot of difference

Originally Posted by jelrod1

I actually get two plates out of the cutter instead of one using this holder over the others.

Seems like you already figured out a decent way to do it. I think it's reasonable to blow through some tooling for a hell job like that. I hope you make some good money off those puppies. Even if you had the worlds greatest set up, I don't think you could expect a cutter to last worth a shit.

You are a hero for taking that job on.

my take is that your issues are centered around, and not in any particular order:
1. coolant/ lube getting to the cutting edge
2.chip evac, unless you have this thing on a bog horizontal and can twist it so gravity sucks the chips out, which is probably not the case
3. the 180 radius at the end of the slot

If you can take a relief cut past the end of the "t" you eliminate the 180 degree buried part. If these are clamping slots like in a press bolster it won't matter if the tnut does not go all the way to the end as long as they can claamp all their stuff. You could also try a hole milled at the end so you don't bury that dog 180 degrees. If you can run with the doors open and an air line full blast evaccing the chips it will help, get a helper and a wetsuit/ scuba mask, because it sucks if ya gotta do it yourself. The wet suit is so you can keep it buried in lube, maybe mix it a little more slippery than recomended, or best case, use an extreme pressure moly based lube. Last, are you using a stagger tooth cutter? makes a huge difference. The last thing I'd do is make 1 pass right down the middle centered first, then run the offset pass at each depth, maybe mixing it up and running down the middle both depths, then run the offsets.

Could you make a pass with a dovetail cutter before the T slot cutter? I am not an experienced machinist so if this is a dumb suggestion ignore it. I like to read threads like this to learn.

All I can think of is cutting as much out as possible with a high performance end mill, then coming back with the t slot cutter. PH Horn comes to mind. They make an awful lot of different sizes with solid carbide shanks. Many different styles of cutters to use also, you can get inserts for it that only have 3 cutting edges, which leave deep gullets for chip clearance. And, for to not make experimentals so expensive, get a sales rep out there to help you. They will let you try it for free. Maybe your customer has some scrap parts that you can use for experimenting with?

Best of luck, takes guts to take on jobs like this.