[pete from TN]

I was looking at the tormach system on the little machine shop website and wishing I had the cash to buy the whole system and starting wondering how it all works and if it would be at all possible to make some holders for yourself. Has anyone ever tried this and how did you do it? I was thinking about buying the small kit with the collet and the setup part and just a few holders and then see if I can make some more from the specs. Whaddya think guys?....peace

[jalessi]

Pete,

Talk to Hoss2006, he made some really nice holders and a kick a$$ air operated power draw bar too!

Jeff...

[project5k]

yea, and dont forget his ATC!

[pete from TN]

Yeah I actually did some searching on the web last night after I posted this and found that he made some and they look very nice. Any idea how he machined them? Were they cnc or manual because they look real nice. I was actually kinda wondering about the possibility of using the mill once it is cnc and machining some from drill rod bar stock by first machining the shank in the lathe for the 3/4inch by maybe 1.75 or whatever they are and then leaving the larger portion and parting off in the lathe. Then taking it over to the mill, inserting it in the mill and using the cnc to accurately machine the rest of the body. I just do not know enough about it to get it done just yet. Seems like if you made them this way they would have to be concentric and spin right in the mill after because they were made in the mill's spindle in the first place. Basically a drilling and boring operation on the vise vertically and then maybe some turning operations for the shape of the body and you're done.... what do you guys think? I know you can but an individual holder for less than 20.00 but if you wanna have a myriad of them around then it could get real expensive no? peace....

[CNCfun&games]

Hi Guy's,

was browsing his thread last nite....Very Interesting stuff!!
look Here:
http://www.cnczone.com/forums/showth...t=43651&page=7

[philbur]

The exterior dimensions are relatively unimportant. The difficult part is getting the tool socket diameter within the correct tolerance and also concentric and parallel to the tool arbor.

Other than that it's a piece of cake.

If you have a lathe then forget about using a mill, CNC or otherwise. You seem to be under the misapprehension that a CNC machine will automatically produce more accurate work than a manual machine.

Phil

Yeah I actually did some searching on the web last night after I posted this and found that he made some and they look very nice. Any idea how he machined them? Were they cnc or manual because they look real nice. I was actually kinda wondering about the possibility of using the mill once it is cnc and machining some from drill rod bar stock by first machining the shank in the lathe for the 3/4inch by maybe 1.75 or whatever they are and then leaving the larger portion and parting off in the lathe. Then taking it over to the mill, inserting it in the mill and using the cnc to accurately machine the rest of the body. I just do not know enough about it to get it done just yet. Seems like if you made them this way they would have to be concentric and spin right in the mill after because they were made in the mill's spindle in the first place. Basically a drilling and boring operation on the vise vertically and then maybe some turning operations for the shape of the body and you're done.... what do you guys think? I know you can but an individual holder for less than 20.00 but if you wanna have a myriad of them around then it could get real expensive no? peace....

[hoss2006]

Philburs right, the most important part is getting the .750 arbor concentric
with the hole for the endmill.
I used a manual lathe with a 4 jaw chuck.
I turned the arbor end with the largest OD too so you know they are concentric.
Flip it around and leave a gap between the toolholder and the jaws so that you can indicate
the toolholder true and then indicate the OD.
Now you can turn the rest of the toolholder.
Drill out the endmill hole about .050 undersize, use a small boring bar to take it within .010 of the needed dia. (drilling alone won't be true enough)
then I used a ream the to take the trued hole to the finished dia.
The endmills slide in with no slop, they actually pop when I pull them out from the vacuum created.
Sounds like a lot of work probably but it's either spend some time or spend some money.
If you could use a collet chuck, it would make the process a lot faster, wouldn't have to indicate each time.
I have the prints and more pics here.
Hoss

[pete from TN]

that the cnc mill would produce more accurate work than manual? I really do not see it in my post after reading it again. The only reason I said that one could use the cnc mill to do the work was so that you could easily repeat the process for several toolholders and they would all be practically the same. I have a 12x36 lathe and have machined some pretty accurate parts on it over the years and obviously this could be done on the lathe but why would you not want to use the cnc and machine the toolholder in the spindle it was made for to ensure that it is gonna be concentric? I do not yet have a collet closer or collet chuck for my lathe but I do have a four jaw and three jaw chuck and a large faceplate.

Hoss I think your toolholders turned out great and they obviously work for you. I am also surprised that you did not make them on your little cnc mill considering your knowledge and ingenious uses of the machine as depicted here. What is your opinion of the system in general? Do you think that it is a good design and does it make the spindle more or less rigid in your machining operations would you say? I know that the repeatability thing is the major attraction for these holders but just wondering about your thoughts now that you have apparently used them for awhile. Have you any tormach ones or did you make everything, did you grind your own collet too? peace....

[cadmonkey]

Though he did say "under the misapprehension that a CNC machine will automatically produce more accurate work than a manual machine" which I don't think really conveyed what he meant well. What I took it to mean (and what I think intended) was that doing it on a mill isn't the right tool to machine a shaft and then a hole on the opposite end concentric and parallel. On a lathe, with the procedure Hoss outlined, you'll get very high concentricity, thus eliminating shaft runout. On a mill you'd be very hard pressed, CNC or manual to keep both ends concentric and parallel with the changing around of parts setup. That's not saying it can't be done, but I'd personally do it on a lathe.

One question for Hoss - did you use carbide/HSS tooling on the arbor or did you use a toolpost grinder? Just curious after my experience with grinding the ballscrew shafts in my conversion.

Greg

[SCzEngrgGroup]

that the cnc mill would produce more accurate work than manual? I really do not see it in my post after reading it again. The only reason I said that one could use the cnc mill to do the work was so that you could easily repeat the process for several toolholders and they would all be practically the same. I have a 12x36 lathe and have machined some pretty accurate parts on it over the years and obviously this could be done on the lathe but why would you not want to use the cnc and machine the toolholder in the spindle it was made for to ensure that it is gonna be concentric? I do not yet have a collet closer or collet chuck for my lathe but I do have a four jaw and three jaw chuck and a large faceplate.

Hoss I think your toolholders turned out great and they obviously work for you. I am also surprised that you did not make them on your little cnc mill considering your knowledge and ingenious uses of the machine as depicted here. What is your opinion of the system in general? Do you think that it is a good design and does it make the spindle more or less rigid in your machining operations would you say? I know that the repeatability thing is the major attraction for these holders but just wondering about your thoughts now that you have apparently used them for awhile. Have you any tormach ones or did you make everything, did you grind your own collet too? peace....

Actually, I think machining the outside, and the endmill bores could be done well on the mill, using a lathe tool and boring bar held vertically in a vise. If you were making several holders for the same size tool, you could program up one, sneaking up on the final bore dimension, then knock off several more in a few minutes. As you said, they should come out nice and concentric, without having to fiddle with a 4-jaw on the lathe. I think it's worth a try. You could absolutely do the outside shaping that way, after turning the shank on the lathe.

Regards,
Ray L.

[pete from TN]

I have run my lathe for years and of course you can machine some very nice and perfectly concentric pieces in it but to be able to make several iterations of the same basic part with little more than a program change would be pretty nice. Now of course if you think it is absolutely necessary to make the final cut with the reamer then you would have a tough time aligning it with the spindle I would suppose. But if it were possible to use a boring bar in the vise that would remain fixed thru the entire operations then it seems to me you should be able to machine a near perfect bore with absolute concentricity only affected by the spindles runout. As I have said before I have NO IDEA how to do this on the cnc yet but I think that once I get my machine running and work out the bugs it would be high on my priority list to do. I think it would basically have to be done with the same setup that has been shown here to make lathe turned parts like the cnc mill to lathe operations posted here and on the youtube. Just then setup basically three tools, a lathe tool, a center drill, a drill chuck, and a boring bar all vertically except the lathe tool of course. Peace.....

[SCzEngrgGroup]

I have run my lathe for years and of course you can machine some very nice and perfectly concentric pieces in it but to be able to make several iterations of the same basic part with little more than a program change would be pretty nice. Now of course if you think it is absolutely necessary to make the final cut with the reamer then you would have a tough time aligning it with the spindle I would suppose. But if it were possible to use a boring bar in the vise that would remain fixed thru the entire operations then it seems to me you should be able to machine a near perfect bore with absolute concentricity only affected by the spindles runout. As I have said before I have NO IDEA how to do this on the cnc yet but I think that once I get my machine running and work out the bugs it would be high on my priority list to do. I think it would basically have to be done with the same setup that has been shown here to make lathe turned parts like the cnc mill to lathe operations posted here and on the youtube. Just then setup basically three tools, a lathe tool, a center drill, a drill chuck, and a boring bar all vertically except the lathe tool of course. Peace.....

Pete,

You've got the right idea. I've used my mill that way a few times, and it's worked really well. One time I made a 12" diameter disc from 3/8" 6061 (for a large disc sander), starting with an octagonal blank I cut in a table saw. It came out perfect, and didn't take long at all. In this case, I think you'd save time by roughing it out on the lathe - drill the endmill hole as close as you can get to final size, then use the mill to do the finishing, taking very light cuts. I'd guess you could do a good job without having to ream. You'll have to write the G-code by hand, but it won't be more than a page of code.

Making some Tormach knock-off holders has been on my ToDo list for a while. I've got a handful of real ones I use every day, and they're great. I'd buy more, but being unemployed for 8 months now, things are a bit tight....

Regards,
Ray L.

[hoss2006]

Pete,
I've used 4 jaws for years, it's about all we use at work so setting up is a snap for me and assures the part is true since you have to indicate.
I whipped out several arbor sides before I switched to the other sides,
loosened the same 2 jaws in between parts so indicating was already pretty close each time.
The tolerances need to be very tight if you want to have accurate repeatability.
I made the arbor dia. and flange width +/- .0005 and the bore concentric within .0005.
I wouldn't trust the mill to hold these tolerances as a vertical lathe, I've seen the videos of mills used like that but with brass or aluminum.
I used tool steel for the holders and it's just easier on a lathe.
I made them all, didn't buy any.
Does your 12x36 have a big bore in the spindle?
you could make your own 5C collet closer.
My 10x22 has MT4 and i've been meaning to pick up some MT4 collets for it but have only found them on Ebay from 800watt.
Whip out a bunch of arbor sides with a 3 jaw then switch to the collet for the
bore sides, no indicating.
Better yet, I just found a new project, an MT4 to R8 adapter but I'll make it for the lathe.
Make use of those R8 collets I don't need anymore on the mill.

Cadmonkey,
I use these carbide inserts, Kennametal CNMG120408P KC730.
Hoss

[philbur]

Sorry, it wasn't meant as an attack but I may have been a bit blunt. However I think you could make ten holders on a manual lathe in the time it would take you to write the program, set up to tooling and verify every thing on your CNC mill. Also your material removal rate on the mill is going to be substantially less than on your 12x36 lathe.

Here’s how I would do it, The process has the advantage that it automatically corrects for any errors in the all important tool socket. Step 8) and 9) is the key. You could perform it on a lathe or mill:

1) Place the tool holder blank in a three-jaw chuck and rough the tool holder arbor and shoulder, center drill the end.
2) Part off (or otherwise) the tool holder blank from the parent material (leave an extra half inch)
3) Repeat steps 1) and 2) for as many holders as you need.
4) Put the arbor end in the three-jaw chuck and machine the outside diameters on the business end to finished size.
5) Drill, bore and the ream the tool socket (don’t forget the extra half inch).
6) Remove the tool holder and drill and tap the locking screw hole on a drill press.
7) Repeat steps 3 to 6) for the other tool holders.
8) Place a suitable piece of bar in the three jaw and machine and polish a mandrel on the end that is a “exactly” the same diameter as the intended end mill. Cut a flat on the mandrel for the tool holder locking screw to seat.
9) Place a tool holder on the mandrel, lock the screw and finish turn the tool holder arbor and spindle shoulder. (use the tail-stock for support, if it’s well set up) Repeat for all tool holders.
10) Remove the mandrel.
11) Place the arbor end of the tool holder in the three-jaw (with protection shims) and machine off the extra half inch your left in step 2).
12) Repeat for all tool holders.

Good Luck
Phil

that the cnc mill would produce more accurate work than manual? I really do not see it in my post after reading it again. The only reason I said that one could use the cnc mill to do the work was so that you could easily repeat the process for several toolholders and they would all be practically the same. I have a 12x36 lathe and have machined some pretty accurate parts on it over the years and obviously this could be done on the lathe but why would you not want to use the cnc and machine the toolholder in the spindle it was made for to ensure that it is gonna be concentric? I do not yet have a collet closer or collet chuck for my lathe but I do have a four jaw and three jaw chuck and a large faceplate.

Hoss I think your toolholders turned out great and they obviously work for you. I am also surprised that you did not make them on your little cnc mill considering your knowledge and ingenious uses of the machine as depicted here. What is your opinion of the system in general? Do you think that it is a good design and does it make the spindle more or less rigid in your machining operations would you say? I know that the repeatability thing is the major attraction for these holders but just wondering about your thoughts now that you have apparently used them for awhile. Have you any tormach ones or did you make everything, did you grind your own collet too? peace....

[SCzEngrgGroup]

Sorry, it wasn't meant as an attack but I may have been a bit blunt. However I think you could make ten holders on a manual lathe in the time it would take you to write the program, set up to tooling and verify every thing on your CNC mill. Also your material removal rate on the mill is going to be substantially less than on your 12x36 lathe.

Here’s how I would do it, The process has the advantage that it automatically corrects for any errors in the all important tool socket. Step 8) and 9) is the key. You could perform it on a lathe or mill:

1) Place the tool holder blank in a three-jaw chuck and rough the tool holder arbor and shoulder, center drill the end.
2) Part off (or otherwise) the tool holder blank from the parent material (leave an extra half inch)
3) Repeat steps 1) and 2) for as many holders as you need.
4) Put the arbor end in the three-jaw chuck and machine the outside diameters on the business end to finished size.
5) Drill, bore and the ream the tool socket (don’t forget the extra half inch).
6) Remove the tool holder and drill and tap the locking screw hole on a drill press.
7) Repeat steps 3 to 6) for the other tool holders.
8) Place a suitable piece of bar in the three jaw and machine and polish a mandrel on the end that is a “exactly” the same diameter as the intended end mill. Cut a flat on the mandrel for the tool holder locking screw to seat.
9) Place a tool holder on the mandrel, lock the screw and finish turn the tool holder arbor and spindle shoulder. (use the tail-stock for support, if it’s well set up) Repeat for all tool holders.
10) Remove the mandrel.
11) Place the arbor end of the tool holder in the three-jaw (with protection shims) and machine off the extra half inch your left in step 2).
12) Repeat for all tool holders.

Good Luck
Phil

Phil,

Unless I'm missing something, you're depending on the 3-jaw to be perfectly true, which most of us can't assume. After machining the arbor andf shoulder, you really want to use a 4-jaw, and carefully zero the part for minimum runout. This is the part that using the mill *might*make quicker and easier if the operator is not very experienced at truing up work in a 4-jaw. No reason the mill can't do the outside profiling just as fast as a lathe, unless it's a little, wimply mill. Writing the G-code shouldn't take long at all - it would only be a few lines of very simple moves - all single-axis moves except for the taper on the outside of the nose.

Regards,
Ray L.

[SSfab]

We have Adjustable 3 jaws on our lathes at work. They are very nice. 9 times out of 10 when you put the work in the jaw, the runout is within .010" then you just adjust and start turning.

[BobWarfield]

I’d with Himy as regards Philbur’s procedure. Don’t think it’ll be accurate. Lots to go wrong there.

Personally, I’d just use the 4-jaw (or my collet chuck which is very accurate and repeatable).

But, I think we can overcome Hoss’s concern about accuracy if we use the mill to CNC the holder. Hoss, I assume your issue is the 2x error issue when cutting diameters and bores? So if your table is accurate to 0.001”, your diameter or bore will only be accurate to 0.002” if you chuck the workpiece in the mill spindle and go from there.

We can get around that.

If you want to machine the whole thing on the mill, that’s doable too, but I’d start out with your 3-jaw on the lathe. Machine the ¾” shank and the nose of the holder, but do not do the flip around to bore the cutter hole or to machine a taper for a drill chuck. Run off a bunch of those blanks. Should be fast and easy. This part would be fine done on the mill as a vertical lathe too, BTW. An error in the diameter of the ¾” shank is small enough the collet can compensate.

OK, now the fliparound. This is the part we worry about because that cutter hole needs to be as concentric as possible with the shank. Plus, as has been mentioned, we want easy g-code. How about doing it all with wizards and short MDI commands? That’s pretty easy.

Grab your spotting (or center) drill, your twist drill of appropriate undersize, and a reamer. You need a way to exactly center these with the spindle axis. I’d use a 5C collet block because I have one and they’re handy. You could probably also press an ER chuck into service. The main thing is you want a low runout holder for your drills and reamer that you can center up and then change the cutters in.

Mount it vertically in your vise and dial it in so it really is vertical and centered under the spindle. Use a drill blank or something else that’s true in the collet to indicate on. Zero the DRO’s on that spot!

Now insert the ¾” shank of the toolholder blank into an R8 collet in the spindle. Center drilling is a 1 liner MDI command. Twist drilling is just the peck drill wizard. The machine doesn’t know the workpiece rather than the bit is moving.

BTW, that hole is dead concentric with the spindle axis. The only issue is the diameter may be a little off because the cutter might be a tad off center. That’s why we use the reamer. It’s got a long shaft so it can float a little bit to seek the hole’s axis. The reamer is another 1 liner. It's not going to got much--just a few thou. Speed and Feed it about 1/3 what you did your twist drill, or even a little less.

I bet you’d find that approach is pretty well dead on. Whether you think it saved you much effort versus the lathe is another question. You could certainly run a bunch of toolholder blanks through pretty quickly this way though.

Use that mill to convert your lathe to CNC and you’re really cooking with fire!

[hoss2006]

I'm not saying it couldn't be done using the mill as a lathe even a "wimpy" mill, but I OWN a lathe so there was no need for me to have to rig up
something on the mill.
If I was going to sell tool holders maybe I would think about it but as Bob said, I would just cnc the lathe.
I only made 2 or 3 each of a particular size, some only 1.
I could make them on the lathe a lot faster.
If you aren't as adept at indicating a 4 jaw, practice makes perfect, but other options have been suggested.
If you want to make tool holders and use the cnc mill then just do it.
There's more than one way to skin a cat.
Hoss

[pete from TN]

As I said I have a three jaw and a four jaw and I know the way to use the both of them pretty well. I have been tinkering in my home machine shop for more than ten years now and have made all kinda cool stuff in there. The three jaw chuck would probably be used to machine the first cut which would have to be the shank and the shoulder. Then part it off. I do beleive that Bob Warfield is on to something here with the collet holder on the mill vise setup vertically. You might even be able to find an accurate ground round short shaft that could be chucked up into the mills spindle and then use the collet closer to clamp a collet of the same size onto the end sticking out of the mill spindle. That way you would be perfectly concentric. Then carefully align the vise and clamp the fixture in the vise. Loosen the closer and raise the millhead watching closely for any movement of the collet edge as you come up out of the collet in the vise. Then you are about as accurate as you might need to machine the holes. This setup has the added advantage of being able to machine the holders with different sized holes for different sized endmills thru a center drill, drill, and ream process. All the while with a carefully setup rigid fixture. The nice thing too is that as long as you do not move the table you would be able to remove the holder and insert a toolbit into it and then test it for runout in the spindle without changing any of your settings. Cnc would only serve to make this a no handle operation and possibly more automated.

Hoss, I appreciate that you made your own and without any dimensions from an original. I guess you just looked at the pictures of them on the net and made your own conclusions about what will and will not work. I respect that and shows how clever you are that you can do it that way. Did you just grind the face of a 3/4 inch R-8 collet to make it work? I think that this project will be high on the priority list once I get this mill converted. I may even start on some before then as I can do them on the knee mill too....

Phil, I am sorry if I came across defensive. I can get that way, I am not the most patient guy and if I offended I apologise. Your input is most appreciated and your knowledge is evident in your posts. Thanks for chiming in on this topic and please feel free to do so whenever you can.... God knows I have much to learn, especially when it comes to this conversion and I am gonna be relying on guys like you, hoss, my buddy art, and Bill on here as well as all of you HSM's for your ideas and interesting points of view. This is a GREAt resource and without it I would have NEVER even thought of trying to build this machine....peace

[philbur]

Note true. It relies on the mandrel you machine while in the 3 jaw to be true, which of course it will be, to the accuracy of your spindle bearings.

The method I describe is well known for achieving concentricity on two ends of a work piece.

The only difficulty it has is if your tool socket diameter needs to be on the small side.

Phil

Phil,

Unless I'm missing something, you're depending on the 3-jaw to be perfectly true, which most of us can't assume.

Regards,
Ray L.