Aloris dovetail dimensions
Close
Login to Your Account
Likes Likes:  0
Results 1 to 20 of 20
  1. #1
    Join Date
    Oct 2003
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,178
    Post Thanks / Like
    Likes (Given)
    71
    Likes (Received)
    121

    Post

    Hi all:
    Can anyone point me to a place where I can get the dimensions for the dovetail slot in BXA size tool holders?
    I bought an original Aloris post and now need an assortment of tool holders to match.

    Also, does anyone have any idea what the tolerance would be on the dovetail?

    Thanks
    Pete

  2. #2
    Join Date
    Nov 2001
    Location
    WAPELLO, IA USA
    Posts
    6,407
    Post Thanks / Like
    Likes (Given)
    29
    Likes (Received)
    1837

    Post

    measure it over dowels, trig out the intersections. draw it up. allow for a sliding fit. cut them yourself. I made some aloris D holders from 7075 that work well for me. I think the genuine ones are probably 1040 or similar.

  3. #3
    Join Date
    Jun 2004
    Location
    titusville fl. usa
    Posts
    3,619
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    16

    Post

    for a $20. toolholder? i think you will have a lot more than that in them making them yourself. if you need a special then i can see that but a bxa is a bxa is a bxa. i know im slow and i sure couldnt have a complete holder in 20 minutes...jim

  4. #4
    Join Date
    Jan 2002
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,314
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    24

    Post

    I posted this write up a long time ago(in two parts..both here), and it is long, but it explains the steps necessary to do the job .
    I have made many holders for special use like:
    1.bored on ends for boring bars (1/4,3/8,1/2)
    2.ball turning tool.
    3.boxtool
    4.indicator holder etc.
    but here is my procedure....

    I have measured both AXA and BXA toolholders from Aloris and will use that information here.
    First, the proper way to measure a dovetail (DT) is with dowel pins a bit smaller than the DT height/depth.
    Normally the pins are layed in the DT and an adjustable parallel is expanded between the pins , and the parallel is then measured with a micrometer . This gives a very accurate dimension.

    The gauge I made was a way of shortcutting this process, but lets follow through the long way first.

    Put the long bar (1.25 X 3X 12"+)in the mill vise and cut a slot for AXA 1.328 wide by .380 deep (1.375 by .418 for BXA) by the length , in the center of the 3" width.
    Cut your 60 degree DT on both sides ,( Roughing cut!) and lay the pins in the groove. measure between them with an an adjustable parrallel or if not available, a vernier caliper. Keep in mind , that the DT cut must be high enough on the wall of the slot so that the .25 pin hits the DT just above its center and is tangent to the DT
    The target dimension is 1.006 between .25 pins for AXA and 1.085 for BXA
    IF YOU GO PAST THIS,THE PART IS SCRAPPED !
    now if you hit it , HOTDOG!, the pins should also be .128 (.166 BXA) from the flat face, which is the top surface as you mill. This you measure down to the pin with a depth gauge, or vernier caliper.
    So now the part can be flipped over and the tool slots cut and then the bar is sawed into pieces.

    But wait , the hard part is hitting the DT and pin dimensions dead on and risking scrap.Also your DT cutter should never drag on the bottom as it dulls the cutter quickly, and lastly, the IMPORTANT dimension is the relationship of the DT to the flat mounting surface.
    So to use this to our advantage, if we make the DT a little deeper (not wider), we have the advantage of hitting the width , then removing the flat surface until it matches the requirement.
    This means that you should mill the slot depth about .010 deeper and also take out another .005 in depth for about an inch wide in the middle so the DT cutter won't cut there.(WARNING Don't make the .005 deeper for the full 1.3xx slot width, as it will screw up your pin measurement !!!!)
    now by starting the DT cutter .010 deeper, if you overshoot the DT pin width, it's not a problem.
    shim the pins on the bottom (say .005) and measure again....if OK, then shoot for the .128 to the flat by milling the flat till it is .128. BINGO, even thought the pins are wider then wanted the part will work perfectly because the RELATIONSHIP TO THE FACE (.128) was held.

    Now since I don't worry about the exact pin spacing results, I made a gauge that has the pin mounted and spaced already and also the .128 dimension to the edge, so when I can stick it into the end of the DT on the bar, it shows me how much to remove from the top flat surface to make a good part.
    This gauge also serves to locate the tap hole locations for the toolholder and I don't have to layout each one. Just dropp it on the toolholder and drill in the drill press.

    Now here is the original post:

    I recently wrote up my procedure for a friend, so I am reprinting it here, since you and maybe others want to make some holders. The following is for the 100 "A" series, so yours should be appropriately larger. Normally, when dovetails are machined, you measure between them with parallel gauges to get the proper dimension. there is a shortcut though as follows:

    No it isn't necessary to grind the holders. You can if you wish, but it does
    not change performance, neither does the type of steel, unless you expect to use it
    over 10,000 times. Hardening is also unnecessary, BUT parallelism of dovetails IS most
    important !

    To start my discussion, take a existing Aloris tool holder and put it down
    on the table with the tool holder part facing you and the dovetail on the
    farside. have the set screws and height adjustment screw removed for our
    discussion. The surface on the far side is what I call the "flats" as it
    goes against the tool post.
    Well , I believe one of the secrets( if you can call it that) is to make a
    gauge from a piece of C.R. or OI 1/4 X 1 x 3 approximately and if it has a
    lip, even better.
    So this gauge will sit on top of the toolholder and the lip should hook the
    far side. The cross-section would be L shaped, but laying down on top of the holder. Now if you
    can, pick it up and the holder and flip over (clamped would help) and drill two holes
    (.2500) against the dovetails for dowel pins- using the dovetails themselves
    as drill guides-you get a doweled jig/gauge that measures the dovetail
    spacing and its distance from the "flats".
    This is important since the depth of the dovetail means NOTHING.
    What's important is the spacing relative to the back (flat ) mounting
    surface, and dowels are the best way of measuring a dovetail and the lip, is the distance. I then press
    in 2 dowels about 1/2" long
    Once the gage is made, I take a bar of 1018 C.R.Steel - 1 1/4 (1" min) X 3" X
    15" or so to make about 9 holders.
    Cut down the center of the bar with a mill equal in width to the dovetail opening
    (smaller dim)or a little larger (doesn't hurt, cause you don't want a sharp
    dovetail edge).
    This would be about (From Memory Now ! may not be exact) 1 1/4 wide by 3/8
    deep by length
    The cut must be deep enough so the dovetail cutter doesn't" hit the bottom"
    same as doing a "T" slot. Take a cut with your 60 Degree dovetail cutter.You should go slightly deeper then a commercial holder.
    Now I lay the gauge on the end of the part and
    hook the lip on the top surface which is the flat, and see if the dowels fit
    in the dovetail.Careful, if the lip is loose, you have scraped the job!
    THERE are 2 ways to go here.
    1>If I want to grind the flats, stop when
    the pins fit , but the lip is lower then the flats ( means I can't hook it)
    If the hook is .002 to .010 short, it means I can set it up on a surface
    grinder and grind down the flats till the gauge slips in.This is what I
    usually do.

    2> If you don't grind, Flycut or face mill the "flats" till the gauge
    fits....LIGHT CUTS,cause the gauge if loose, means that the holders will be
    sloppy.( One of the reasons that the tool post handle is not at 4 O Clock as it
    should be when clamped

    Once the "bar has the right dovetails, I flip it over and layout the 1/2 X
    1/2 tool slots using a holder as a guide, and machine them a right angle to
    the bar...fast this way...then saw cut them out.
    Then I clamp my Aloris Tool Post "t" nut in the milling vice, and mount my
    tool post to it,making sure it is plumb. Now put the holders in the post
    where wanted and mill the tops, and flip and do the bottoms.OR you could put
    a piece of 1/2 X 1 into the slot and set it on the vice jaws and mill also
    without the post.
    That's it....except I didn't tell you about my gauge exactly.... it has the
    dowel pins and I don't have a lip, but eyeball it, and I also have the layout for
    all 4 clamp screw holes and the height screw hole. these are tap drill hole sizes
    , so I can take a new holder and set the jig on top and drill the holes in
    the drill press...the dowels hold it in place.
    To finish, I belt sand them lightly to remove tool marks but watch...no
    tapered grinds,break corners and then use Birchwood Casey Tool Black and
    they look good.
    In the past , I have made the Height screw knurled knobs etc. The last batch
    got real Aloris adjusters....MSC sells them for about $5.50 nuts/screw/washer as a
    kit and the are the nuts !

    If you feel nervous about the Dovetails , just cut the end of the bar in about 1" and keep using the gauge till you get the right cross slide settings. Also try to cut one DT completly through and sneak up with the other side,so you don't have two variables.

    One last thing, any left over piece from the bar is not tossed. I have a 3/4
    inch high boring tool holder ...drilled for a 3/8 boring bar
    And one a 1/2 high for a dial indicator mount...who says they have to have
    open sides!

    have fun and hope this helps

  5. #5
    Join Date
    Sep 2002
    Location
    northeast
    Posts
    1,721
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    7

    Post

    Rich,
    FYI, I posted this a little earlier this evening on the HSM forum. I measured 2 BXA holders tonight, one brand new and one older but barely used, both Aloris.

    One measured 0.750" between 0.375" dowels and the other measured 0.742" between the same dowels. The older holder puts the handle at 6 o'clock (perpendicular to the Aloris name plate). The new one puts it at 5 o'clock.

    I've heard of variation in the Aloris before and this demonstrates some of the range.
    Den

  6. #6
    Join Date
    Jan 2002
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,314
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    24

    Post

    Den
    I layed it out in Autocad and see that
    my original dim for BXA is about .0014" wider than your .742, and of course your .750 is wider than mine by .0066

    I did this to corrolate the difference between the .250 pins and the .375..

    I would think that the .008 range you have is a little bit wide, but within reason on a production basis.
    I have some BXA holders, but no post, so I cannot evaluate the position of the handle .
    Almost all of my (stock) AXA's are at 4:30 when tight ?..and on both Aloris posts (2)

  7. #7
    Join Date
    Sep 2002
    Location
    northeast
    Posts
    1,721
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    7

    Post

    Rich,
    A while back on the Chaski board, Marty had some dealing with Aloris over some holder / toolposts that would not mate.

    I've got a feeling that 0.008" is not the end of it If you're curious, I can measure some more as I've got about 10 or so spanning about 25 years. All are very lightly used so there should be negligible wear.

  8. #8
    Join Date
    Oct 2003
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,178
    Post Thanks / Like
    Likes (Given)
    71
    Likes (Received)
    121

    Post

    Rich:
    Thanks for the fabulous post!! Lots of information, I think that I will be able to get myself into lots of trouble with that much

    Den:
    I'd love to hear the result of your measurements. It would give us some idea of the "allowable" tolerance on the dovetail.

    Cheers
    Pete

  9. #9
    Join Date
    Dec 2000
    Location
    Bremerton WA USA
    Posts
    10,673
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    4228

    Post

    Be careful of what you use for a reference when taking pin measurements over dovetails. Be sure it's the faying surface. It's easy to lay the pins in the male dovetails and take a mike reading but the female DT will have depth clearance and the pins will into not automatically fit precisely flush with the reference surface.

    Problem is, you need to have a way of holding the pins tight to the reference face of the female DT and measuring the opening between the pins with an adjustable parallel or mike over the pins where they extand past the DT. This can be tricky to do without making a few machined inspecion aids that positively force the pins flat against the reference face and the DT flanks.

    For this reason I usually suggest that DIY tool post accessory makers purchase at least one factory toolholder to use for a set-up piece.

  10. #10
    Join Date
    Jun 2004
    Location
    titusville fl. usa
    Posts
    3,619
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    16

    Post

    the use of adjustable parallels is the way i measured my aloris toolholders i just wish my wire edm guy wasnt so busy and he would finish the axa to bxa conversion...jim

  11. #11
    Join Date
    Nov 2001
    Location
    Bentley, Louisiana
    Posts
    3,384
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    15

    Post

    Like Mr. Addy said, with female dovetails, the surface is the key. This sets the distance and the "clock position" of the toolpost's handle.

    As a side note, I've found that there is variation of dovetail measurement between different brands (Aloris, DTM, Dorian, etc), and they're surprisingly big I can tell you, and they're all intended for the same series tool post.

    Good luck,

    Richard

  12. #12
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,871
    Post Thanks / Like
    Likes (Given)
    3599
    Likes (Received)
    3023

    Post

    Interesting that the dimensions are all over the place yet all the major manufacturers swear they'll repeat within a half a gazillionth of a nano-meter

  13. #13
    Join Date
    Sep 2002
    Location
    northeast
    Posts
    1,721
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    7

    Post

    metlmunchr: They do repeat and it is a function of the surface finish of the toolpost, dovetails and slides, not the absolute dimensions. That's where hardened and ground holders work best.

    Here's a summary of the 12 holders I have which span about 25 - 30 years of manufacture. They are in the order measured because I am lazy at this hour:

    All were measured between two 0.250" (actually 0.2501, 0.2499) ground rods using an adjustable B&S parallel: (Note that the bottom of the female dovetail is not flat but has 2 ground mating flats with the central region of the surface being a little deeper for clearance. These measurements are only to the ground surfaces)

    1.092 1.082
    1.081 1.087
    1.084 1.087
    1.085 1.083
    1.086 1.086
    1.086 1.084

    The distribution looks centered near 1.087 and a +/- 0.005" tolerance would absorb all of these.

    Den

  14. #14
    Join Date
    Aug 2004
    Location
    San Jose, CA
    Posts
    596
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    metlmuncher, Isn't that what the wedge is about? The distance can be within a range, but the wedge will still contact it, and it will be repeatable as long as the mating surfaces are coplanar and flat?

    I don't pretend to be an authority, but I thought that that was the purpose of the design--to ensure repeatability without requiring ridiculous tolerances.

    Justin

  15. #15
    Join Date
    Jan 2002
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,314
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    24

    Post

    Hey Wait a minite Guys !
    Don't get excited about loose pin measurements !
    You are missing the point..bigtime .
    ( Den, I need to read what Marty found out )

    Getting the dimension between the pins is only HALF of the requirement !
    Note I said earlier:
    "cut a slot for AXA 1.328 wide by .380 deep (1.375 by .418 for BXA) by the length , in the center of the 3" width"
    (This is with a ordinary 2 flute endmill !)

    If your depth is greater than .380 (or .418 BXA), the dowel spread must be "Greater" and the part Can/will still fit fine ! Thats why I pointed out the face of the holder, which rests against the toolpost, before the wedge even comes down
    The dovetails could be 3 inches wide at what ever depth you have..but the important part is the space between them at the point where they meet the face, for mounting to the wedge.
    Put another way( in Simple Terms), You need to machine the DT and measure the gap at the face , which is the closet point of the angles...BUT that is not practical ( burrs etc)and not good practice in our trade ! So you go to a Known depth (ie.380)
    Only by holding the roughing depth to .380, can you come in with a DT cutter , touch bottom , and expect to hit your target dowel pin spread dims mentioned!
    Forrest is correct about the difficulty of using parallels, but the way to do it is to extend the adjustable parallel beyound the top of the holder, spread the pins tight and mike it THERE, not to remove and measure!

  16. #16
    Join Date
    Sep 2002
    Location
    northeast
    Posts
    1,721
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    7

    Post

    Rich,
    If I digested half of that, measuring between the dowels would only be valid if the "depth" of the female dovetail is consistent.

    A quick check of 3 holders shows 0.4192, 0.4172, 0.4143 ... not all that tight.

    I did spread the adj. parallel firmly against the dowels and mic'ed across it but I think what Forrest is saying is that we really want the dowels against the plane of the outside flat of the dovetail and not the inner face? This is because that outside flat is pulled against the toolpost.

    So, the toolholder should be layed on a surface plate, dowels spread inside the dovetail BUT also held against the surface plate?

    I think I can see why Aloris had difficulties at least once

  17. #17
    Join Date
    Jan 2002
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,314
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    24

    Post

    Yes Den...you said;
    "So, the toolholder should be layed on a surface plate, dowels spread inside the dovetail BUT also held against the surface plate?"

    You got it !..and that is exactly what Forrest meant, because that is the proper method used in good "machinist" practices...BUT

    Most folks here don't have surface plates.
    Most folks have never measured "V"s before.
    Most folks want to try to measure with a "valid" style while still in the machine, to save time,and yet achieve some accuracy .

    I tried to address those issues with the method I pointed out..
    By the way, for the benefit of our readers here ,what I called the "face", you call the "Outside flat". no problem...

    Summary;
    Since the face is critical,but not available as an easy surface to check, you must machine to a "constant" parallel depth as a reference point in order to measure with dowels ,with my method..that simplifies the issue for the work.
    A guy could also make the gage I mentioned , which does look at the outside flat as a source of control..

    Den . the depth comparisons you found show a variety of depths ,as you pointed out, but Aloris probably pays no attention to them, because they use methods outlined by Forrest.The bottom of the DT is really an "air fit" in real life, but very important for manufacturing with my method

    A very easy way (but time consuming !) to find the right distance, is to machine close, then put your post up to the work and check, and take a few thou off, and recheck

    den, Thanks (!)for clarifying our discussion.
    I'm sure some folks here learned a few things

  18. #18
    Join Date
    Sep 2002
    Location
    northeast
    Posts
    1,721
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    7

    Post

    Rich,
    I do hope that it may have helped someone else and that my confusion wasn't just eating up bandwidth
    Den

  19. #19
    Join Date
    Oct 2003
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,178
    Post Thanks / Like
    Likes (Given)
    71
    Likes (Received)
    121

    Post

    Rich, Den, Forrest, etal:

    I was able to spend a little time in the shop this morning, and I put a little of what you told me to work.

    I modified some shop made AXA holders to fit the BXA post I have now. This is a stopgap situation, but will suffice until I acquire some of the correct material.

    In re-cutting the dovetails I noticed the following:
    The import BXA blocks I have fit very nicely with the handle locking in the 4-5 o'clock position. The dimensions on both of these blocks are 1) depth 0.418" 2) width at the opening of the dovetail 1.375" 3) measurement between 1/4 pins is 1.075" Both blocks are very close.

    I tried to get the shop made blocks close as close to these dimensions as I could, subject to what I had to work with. I noted that 3 of the 7 blocks I re-cut would not fit on the post despite being fairly close in dimensions to the samples.

    Applying the information that Forrest gave regarding the the contact surfaces, I placed one of the holders on the surface grinder and removed a couple of thou. BIG difference!! So I proceeded to grind each block, on a cut-and-try basis so that each would fit easily and lock with the handle at the 4-5 o'clock position.

    I found that once the block slid onto the post, I was able to move the position of the handle 10* for every .001" removed by grinding.
    A nice side effect of the grinding is that the blocks slide onto the post much more smoothly.

    When I get some more material, I am going to make a gage, as suggested by Rich, but I think that I will make a small change in his process, in that I will grind the surface of the blank first, and have a lip that will position the dowels at the correct height fron the mating surface.


    Thanks for all the advise
    Pete

  20. #20
    Join Date
    Jun 2014
    Location
    NE Ohio USA
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    7

    Default

    Hello,
    Yes, I do realize that this thread is about to go the way of the dinosaurs. If a person reads these replies, they will possibly encounter some confusion.
    There was quite a lot of discussion about some variation of the dimensions inside the dowels. That is fine. If the dimensions allow for a tight clamping to the tool post you are fine. Let us assume that we have a lathe with digital read outs on it, with the capability to set offsets for each tool.
    Personally, I prefer to number each holder with a paint marker to allow the use of a holder for a different position on another job. Insert and clamp all of the tools into the holder blocks and clamp them tightly. From now on, the set-up is simple. touch each tool to a known Z axis datum face, and an X axis diameter, and set the offsets on the DRO unit.
    The point that was either missed, or not mentioned, is that each assembly of tool and holder has its own identity. Any slight variation of depth or width of the dovetail plays no part once the set up is complete. Each holder will be forced into battery against the face of block, and the leading side of the dovetail within tenths.
    If you are running multiple parts, the first "tool" can be a piece of steel clamped into holder"1". This tool can be set-up to read "0","0" when in a position to allow sufficient stock for a clean up on each piece to follow.
    Hopefully no one will find this explanation "confuzicating".


Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •