PDA

View Full Version : I want to make CA and AXA tool holders



rsr911
09-16-2006, 12:32 AM
As the title says i want to make a bunch of CA (for the big lathe) and AXA holders for my little lathe. The plan is to do this on my CNC and I've got a few questions as to a good procedure. I've got long stock of roughly the correct cross-section and I was thinking to first face all four sides then cut the dovetail slot lengthwise down the piece. After this I would cut the block blanks on my hacksaw, set the blanks up in soft jaws in my vises dove tail down, square up the saw cuts and mill the tool slots. I could then flip them 90 degrees in the soft jaws and drill the holes for the set screws and height adjustment. I'll need to do the tapping on the manual mill as I don't have a NMTB #30 tapping head (wish I did!) Any thoughts? How would you guys do it? What about DOC and speeds and feeds for a dove tail cutter?

TIA

-Christian

lazlo
09-16-2006, 12:40 AM
Ask what kind of steel to use. I dare you... :D

rsr911
09-16-2006, 12:48 AM
Ask what kind of steel to use. I dare you... :D


Nope, just whatever junk I picked up at the scrap metal dealer LOL :D

TGTool
09-16-2006, 11:27 PM
Sounds like a reasonable approach to me. I've made several AXA one-offs, so the proposition of doing the dovetail on the whole stick seems good. For manual machining, after milling the rough stock out in the center of the dovetail I typically take two rough cuts and a finish cut to size on each side with a 1-3/8 dovetail cutter IIRC.

Jan

wierdscience
09-16-2006, 11:31 PM
I don't know,but we have a foundry here local that does cast steel,guess how I'm going to make my next hundred?:D

Rich Carlstedt
09-17-2006, 01:47 AM
I have made mine by milling the dove tail down a 12 inch bar(s) as you stated.
However, i flipped the bar and did all the cross slots (tooling groove) after the dovetail work. Then i sawed the bar to give me the holder heaight + some for cleanup (2 sides), Then I mounted my ALoris Tool Post right on The Mill. dropped the holders onto the toolpost and clamped them . had a 1 inch high stop under the holders and then faced them all. flipped them over and did the final face, then drilled the holes and tapped them all while in the tool post.

End cuts from the bar like 1" high are not thrown away. They are bored for mounting boring bars (ie,3/8" 1/2" or 1/4 "for indicator shafts)

Dovetail cutter..blow air into the cut..it's the chips coming back round that break the teeth !

Last tip.
Buy your Aloris adjusting screw and stop "kits" right from MSC.
You get the 2" long thread screw with nuts and knurled knob cheap
Rich

rsr911
09-17-2006, 02:42 AM
I like that idea of mounting the tool post right on the table!

I'm gonna just put two or three blanks in each of my two vises with notches cut in the soft jaws. I have programs for soft jaws for the CNC vises, manual vise, as well as for the 3 jaw chucks for the large and small lathes. I just put in my reference jaws, clamp in the stock and let the mill do the work. Currently I have two unused sets for the CNC. I figure I'll make about 20 toolholders for each lathe. Thanks for the tip on the height screws, I'll check on it. :)

Mark Hockett
09-17-2006, 03:16 AM
Christian,
Cutting the dove tail first on long strips is a good way to make the holders. Then saw cut the rough holders. You could then make some soft jaws for your mill vise with a dove tail on top and on each end, this would hold the parts by tightening the vise in reverse. Place stops on 2 positions on top and height stops on the sides. This way you can do 2 holders at a time or maybe 4, 2 on top and 2 on the side, if the vise will tighten up on all 4 holders. Use the top for for squaring up the ends and cutting the tool grove and use the sides for drilling and tapping the holes. Write a program that will do both operations and that way 2 finished holders come off the machine each cycle. I have made hundreds of tool holders for the TS post used on the mini lathes.
http://i24.photobucket.com/albums/c10/mahockett/thred.jpg
http://i24.photobucket.com/albums/c10/mahockett/thblue.jpg

Millman
09-17-2006, 06:23 AM
Mark, yours are too damn fancy. I like the look! A toolholder of any dimension is only as strong as what it's attached to. Made some toolholders from soft brass and they also provided a dampening effect of vibrations for certain applications. Don't fret about the materials for the toolholder, because your cutting tool has only a thousand variables involved right at the point of contact. Just use what you have.

John Stevenson
09-17-2006, 06:53 AM
Clean all 4 side if you can't get stock the right size.
Cut the dovetail in one long strip.
Saw into blanks.
This will leave bottom and top rough and minus the slot and drilled holes.

You may want to ignore the bottom or linish, after all no one sees it and it doesn't do anything, your call.

Then fit the holder to a dummy strip mounted in a dividing head / indexer with tail stock. Set so the dovetail is vertical and mill the top face, index round 90 degrees and do the slot, index back 90, change tools and drill the holes.

Job done on one setting.

If you want to clean up the bottom it's another 90 index before you swap for the drill.

.

Forrest Addy
09-17-2006, 08:29 AM
Dovetail cutters are delicate. The teeth are seldom concentric with their shanks and that little skinny neck is a great place to break them if you try to over load them. You won't make the dovetail cuts in a single pass. Take 2/3 of the stock the first cut, all but 0.010" the second and the balance to pin size on the third. You will be able to feed 2 to 5 IPM at 70 ft/min (300 for aluminum) dependiing on the eccentricity of the cutter. A cutting oil spray mist that blows chips clear is an excellent proposal.

Making the blanks as a bar of common cross section then cutting them to height on a cut off saw only makes sense.

I'd make tool holders from prehard material but the lowball crowd have some justification in making them from mild steel or aluminum. If you are going to mak any make a bunch. Two dozen at a time isn't out of reason. If you make them well of good material you can get a good price for your surplus holders. Leave a few oversized and blank against the time you might need one to make a little tool post grinder or milling/drilling head.

rsr911
09-17-2006, 11:17 AM
Looks like you guys have done it similar to the way I'm proposing. Although a few ideas like dovetails on the soft jaws or using a rotary table don't make much sense in my application. Here are my proposed steps.

1) face side of stock
2) face opposite side of stock
3) face top of stock
4) face bottom of stock
5) rough out dovetail with endmill
6) machine dovetail
7) powerhack saw toolholder blanks to height + cleanup material
8) place blanks in soft jaws dove tail down with sawcuts perpendicular to jaws.
9) using a long endmill cleanup what will be the top and bottom of the holders and machine the slots
10) flip holders 90 degrees in the vises and drill holes for set screws and height adjuster.

Of course I'll do step 9 to all the holders before moving to step 10.

Forrest, thanks for the feeds/speeds for the dovetail cutter. I've just got to pick up a few large endmills so I can get started. I'm gonna use a 1" endmill for the facing work and roughing out the dovetail. I'll be doing the CA holders first as I need more of them right now.

Chuck U&R
09-17-2006, 11:23 AM
I registered here a long time ago but haven't posted in forever !
I drop by once a week or so to pick up whatever little tidbits of infomation I can.

Anyway - I just bought a 12x36 lathe and a Phase II series 200 (BXA I belive) QC toolholder.
Is anyone willing to cut dovetails in a couple pieces of mild steel for me so that I can make some extra toolholders ? Say 2 pieces 11" long each.

Of course I'll pay and I'm sure I can do everything else I just don't have a mill to cut the dovetails - yet.

Thanks.
Chuck U&R - upandrunning at mindspring dot calm.

Forrest Addy
09-17-2006, 11:35 AM
Chuck, if you can mill you can cut dovetails. The cutter does the hard part - making the internal angles. Use care because the cutter is a bit fragile but otherwise just a milling cutter.

The only trick is to get the size right and for that you can use the tool post itself as a gage.

lazlo
09-17-2006, 11:41 AM
Chuck, if you can mill you can cut dovetails.

I agree with Forrest -- cutting the dovetails on a BXA is a great learing experience.

Just cut the main slot with a conventional endmill, and save the dovetail cutters for the final angle cuts.

Chuck U&R
09-17-2006, 11:43 AM
I don't have a mill.
I'm thinking that once the dovetails are cut I can mount the toolholder on the QC post , chuck up an end mill and cut the toolholder slots on my lathe.

I know that I can buy these for $16. each but I think it would be good experience to make them myself and hopefully save some $$$$.

Thanks.

billr
09-17-2006, 12:55 PM
it might help some if you would tell us where you are.

peace.
billr.

Chuck U&R
09-17-2006, 01:24 PM
Sorry - I'm in NC, near Pinehurst. About an hour south of Raleigh.

I really wasn't thinking about location since the post office has those flat rate boxes. Fill 'em up for $8.-$9.

rsr911
09-17-2006, 04:52 PM
Chuck,

I can certainly do it for a good price for you but I need the dimensions for a BXA holder. My email is in my profile, email me so we can discuss off board.

-Chris

Chuck U&R
09-17-2006, 07:25 PM
Thanx for the response -
I'm going to the post office tomorrow to see what can fit in a flat rate box.
I'll E you offsite with dimensions and quantity.
Thanx !

Chuck U&R
09-18-2006, 04:27 PM
..........

rsr911
09-18-2006, 10:04 PM
reply sent. I also ordered a 1 3/8" dovetail cutter today to do the CA toolholders.

rsr911
09-21-2006, 03:27 PM
Dovetail cutters are delicate. The teeth are seldom concentric with their shanks and that little skinny neck is a great place to break them if you try to over load them. You won't make the dovetail cuts in a single pass. Take 2/3 of the stock the first cut, all but 0.010" the second and the balance to pin size on the third. You will be able to feed 2 to 5 IPM at 70 ft/min (300 for aluminum) dependiing on the eccentricity of the cutter. A cutting oil spray mist that blows chips clear is an excellent proposal.

Making the blanks as a bar of common cross section then cutting them to height on a cut off saw only makes sense.

I'd make tool holders from prehard material but the lowball crowd have some justification in making them from mild steel or aluminum. If you are going to mak any make a bunch. Two dozen at a time isn't out of reason. If you make them well of good material you can get a good price for your surplus holders. Leave a few oversized and blank against the time you might need one to make a little tool post grinder or milling/drilling head.


If I use the cutter max OD of 1.375 with a SFPM of 70 I get 194 RPM and 5 IPM. Should I feed slower? Also would it be better to conventional mill or climb mill?

rsr911
09-22-2006, 12:46 AM
Hmm,

I've looked everywhere and I can't seem to find a chart for feeds and speeds for a 1.375 dovetail cutter. I also can't determine if climb milling would be best (for chip removal) or conventional (to reduce cutter flex). Anyone have any suggestions? Forrest's numbers look good but he didn't specify the cutter size so I don't know if he assumed I'd use a 1.375 cutter or not.

TGTool
09-22-2006, 10:40 AM
Christian,

Your rpm calculations are good (yesterday's post). Use conventional milling only unless you do a last pass for surface finish with only about .001 cut. In my experience, conventional milling has left a perfectly good finish. In any case, the finish on this inside dovetail isn't a big issue since this is just a position-and-clamp application. If it were a machine slide for fine positioning it would merit more attention.

Jan