[digits]

Hi guys, I need to make some largish aluminium parts with 2-3" deep pockets, and I'm looking for some TTS compatible way of hogging out their innards.

I currently have very long 100mm (4") 10/12mm end mills in TTS set-screw holders, but ideally I'd like something stiffer.

Does anyone know of a TTS compatible tool that would do the job at a reasonable price?

The Tormach modular insert stuff looks like it might work - but I can't tell from the data sheet what the diameter the shafts on the holders are. They'd need to be smaller than the heads to allow deep work. It's also rather expensive IHMO - and I can't seem to find any reviews of them on here.

Cheers.

[GLCarlson]

You might take a look at the Glacern EM90-750B with APGT1135 inserts. It's not exactly what you were looking for, but a TTS ring added to the 3/4 shaft gets one a "TTS compatible", and it's one piece. The shaft is about twice the circular area of a 12mm tool (that is, twice as stiff). Can mill to 3" depth. I've got one, like it. My only problem with it is that it's another bloody insert to stock.

I've looked at the TTS thread-on cutters. Seem to be Mitsubishi sourced, and as you note, expensive unless used for production.

[Steve Seebold]

First off, there is no way I would try to mill a pocket 2 to 3 inches deep. I would create a hole pattern and drill most of the stock out then use your end mill or whatever cutter you choose to finish the sides and bottom.

Depending on the size of the pocket you need to make, it could take hours to make it that deep with an end mill, but you could drill it out on minutes.

If you want to use a 3/4 inch end mill, fine, use a drill to make a 3/4 inch hole, then use your 3/4 inch end mill and make .200 stepovers to plunge ruff and you'll move more material than you ever would by side cutting with an end mill.

I know it works, I have several repeat jobs that I do this way. One particular job takes 36 minutes to side cut with an end mill, and it takes 11 minutes to plunge ruff and finish, and I do it all with the same cutter.

[digits]

You might take a look at the Glacern EM90-750B with APGT1135 inserts. It's not exactly what you were looking for, but a TTS ring added to the 3/4 shaft gets one a "TTS compatible", and it's one piece. The shaft is about twice the circular area of a 12mm tool (that is, twice as stiff). Can mill to 3" depth. I've got one, like it. My only problem with it is that it's another bloody insert to stock.

I've looked at the TTS thread-on cutters. Seem to be Mitsubishi sourced, and as you note, expensive unless used for production.

Thanks - the Glacern mill looks interesting, but by the time you've bough a box of inserts, you're out $250 odd...

How does the TTS conversion collar work on a tool with a parallel shaft and no obvious step to glue it to? What stops the drawbar force breaking the glue?

[digits]

First off, there is no way I would try to mill a pocket 2 to 3 inches deep. I would create a hole pattern and drill most of the stock out then use your end mill or whatever cutter you choose to finish the sides and bottom.

Depending on the size of the pocket you need to make, it could take hours to make it that deep with an end mill, but you could drill it out on minutes.

If you want to use a 3/4 inch end mill, fine, use a drill to make a 3/4 inch hole, then use your 3/4 inch end mill and make .200 stepovers to plunge ruff and you'll move more material than you ever would by side cutting with an end mill.

I know it works, I have several repeat jobs that I do this way. One particular job takes 36 minutes to side cut with an end mill, and it takes 11 minutes to plunge ruff and finish, and I do it all with the same cutter.

That is a good point - it would be very slow side milling away 5kg/10lbs of metal...

Have you got any video of your pluge milling in action? I've never seen it done on a relatively lightweight machine.

[Steve Seebold]

That is a good point - it would be very slow side milling away 5kg/10lbs of metal...

Have you got any video of your pluge milling in action? I've never seen it done on a relatively lightweight machine.

I don't have a video right now, but I have a repeat job that requires plunge ruffing that I will be running in the next 2 to 3 weeks. I'll get some video then and post it.

For the job I am going to plunge ruff, I use a 1/2 inch 2 flute end mill with a .060 radius at 4,500 RPM. When I do the slotting cuts (full width of the end mill) I use a .150 stepover and a 25 IPM feed rate, then when I get out of the slot I increase the stepover to .225 and the feed rate to between 30 and 40 IPM. Trust me, it fills up the chip bucket in a hurry.

I make my program so I leave .015 to .020 stock for the finish cut.

Try it and you'll never side mill a pocket again. I also use this method when I have a lot of material to remove from the outside of a part.

[GLCarlson]

Re cost. It is indeed the thick side of 3 bills. I got mill and inserts on sale, probably wouldn't have done it otherwise.

Next let me agree with Steve S. Drilling and/or plunge roughing is the way to do this.

That said, my approach to the TTS is to make shrinkfit collars out of 4140 HT when I have a compatible shaft. Someone else reported using 7075 Al in an earlier thread. I don't have a PDB (yet), so I'm hand tightening-haven't seen a problem. Don't have any experience with the actual Tormach product, and should have made that clear. My excuse is that it was early, and I was insufficiently caffeinated while typing.

[Scott_M]

That is exactly the type of machining operation the modular tooling was designed for. You get a very rigid extension with the option of changing the heads. I am not sure what info you saw but they do have a good pdf with specs. It can be found here. http://www.tormach.com/uploads/51/DS...0212A-pdf.html The diameters of the shank on the M8 is .565" and the M10 is .725" The dimensions for the cutter heads are in the pdf.
It is a nice elegant solution for your problem.

Scott

[David Bord]

I purchased the Tormach 17mm center cutting insert EM and am super impressed with the metal it removes.

You can search my name for a post I made on it with a video.

[Steve Seebold]

Here is a short animated video from Sandvik to show what I am talking about to plunge ruff your pocket.

http://www.sandvik.coromant.com/en-u...s/default.aspx

[David Bord]

Steve, it seems that I have trouble doing plunging with EMs, as the machine shudders unless I go very slow. I have less of an issue using drill bits, but I normally use a deep drilling cycle at any depth. Maybe a chip clearing problem?

With that said, I haven't done much if any partial width plunges, so that may be part of the issue.

Not sure if it's my technique, or something with my machine.

I have not tried center cutting with the new insert em I purchased from Tormach, that may work better.

Any tips would be appreciated.

David

[Steve Seebold]

Steve, it seems that I have trouble doing plunging with EMs, as the machine shudders unless I go very slow. I have less of an issue using drill bits, but I normally use a deep drilling cycle at any depth. Maybe a chip clearing problem?

With that said, I haven't done much if any partial width plunges, so that may be part of the issue.

Not sure if it's my technique, or something with my machine.

I have not tried center cutting with the new insert em I purchased from Tormach, that may work better.

Any tips would be appreciated.

David

If you're plunging into a part, I would do it with 2 tools. First use a G83 cycle to drill a hole so your end mill has a place to go, then change to your end mill. An even faster way would me to use a large drill and use a large enough step over so the drill doesn't break through into the previous hole.

If you'd like, send me a .dxf file of your part, the pocket depth, and the corner you're starting from, and I'll send you a program that will work the way I would do it. Don't forget to tell me what size end mill you will be using and whether it's HSS or carbide.

[MichaelHenry]

Steve, it seems that I have trouble doing plunging with EMs, as the machine shudders unless I go very slow.

Are you using center-cutting end mills? If not, you won't be able to properly plunge mill through solid stock.

Mike

[Steve Seebold]

Are you using center-cutting end mills? If not, you won't be able to properly plunge mill through solid stock.

Mike

:cheers:Yes, I ALWAYS use center cutting end mills. BUT, if I am doing a pocket, I will use a drill that is the same size or 1/64th larger than the end mill I want to use first. There is no tool in your arsenal that will remove pocket material faster than a drill.

I will make a drilling program with a step over that is .015 to .030 larger than rge diameter of the drill. That way, your drill won't deflect in to the hole next to it. When you have all the material drilled out, then make another program with a smaller step over and use your end mill to get within .010 to .015 of the walls and bottom, then it's easy to finish your pocket.

If you're making a pocket that's a half inch deep and using a 1/2 inch drill, you can probably use a G81 drilling cycle. If your pocket is deeper than that, then I would use a G83 and a peck that won't load up the flutes of your drill.

I said earlier, if you can send me a .dxf or a solid model in one of the following formats parasolid .x_t, .igs, .stp, .sat of the part you want to do, I'll make you a program to show you how I would to it.:cheers:

[MichaelHenry]

Steve, I try to use centercutting end mills, too, but thought David might not be. That could explain the shudder he sees.

Mike

[David Bord]

Hey Steve,

Thanks... using a drill first makes more sense for the intial removal. I really appreciate the offer to do some code for me. I dont have a project that I am working on currently that falls into this area. It was a general question since ive had challenges plunging in the past with EM. Clearly a drill will solve that.

Mike, yep, definately using center cutting EMs so thats not the issue. I have a feeling its a chip clearing issue and I assume square EM arent a great solutioin for doing a intial entry plunge at any speed on a light machine?

David

[shred]

Plunging full-width directly into solid material with a center-cutting end mill is somewhat problematic on smaller machines as the effective SFM at the center of the tool approaches zero. So what the end of the cutter 'sees' is effectively a hard spot in the center fading out to easier cutting. The cutter tries to move in the direction of the easier-to-cut material, only to have the machine, tool holder and tool shank drag it back into line. If there's any lack of rigidity in the system, then you get shuddering and oversize holes as the cutter end orbits around trying to go in the direction of the easier material location while being dragged back to center by the machine.

[Steve Seebold]

Plunging full-width directly into solid material with a center-cutting end mill is somewhat problematic on smaller machines as the effective SFM at the center of the tool approaches zero. So what the end of the cutter 'sees' is effectively a hard spot in the center fading out to easier cutting. The cutter tries to move in the direction of the easier-to-cut material, only to have the machine, tool holder and tool shank drag it back into line. If there's any lack of rigidity in the system, then you get shuddering and oversize holes as the cutter end orbits around trying to go in the direction of the easier material location while being dragged back to center by the machine.

That's exactly why you start with a DRILLED hole

[digits]

That's exactly why you start with a DRILLED hole

Can I ask what size drills and mills you are using?

I tend to use bigger diameter mills than drills myself, and so just drill out a small hole and then spiral down into it with an end mill.

[Steve Seebold]

Can I ask what size drills and mills you are using?

I tend to use bigger diameter mills than drills myself, and so just drill out a small hole and then spiral down into it with an end mill.

I will use a drill that is either the same diameter as the end mill or 1/64 larger. And I will use a step over that is one diameter plus 1/64 so that the next hole doesn't drift into the hole before it.