# Advice for Dove tail Milling First Time



## jlsmithseven (Mar 26, 2017)

This is our first time dovetail slot so I am going to go slow. Any advice would be awesome. Thanks guys!


----------



## ddickey (Mar 26, 2017)

Couldn't you use two different sizes and use the average in your calculation?


----------



## Bob Korves (Mar 26, 2017)

You can use two different size gage pins for measuring across dovetails as long as you use the same ones for every measurement.  I would try to find two that are as relatively close as possible in diameter.  The pins will of course need to clear the dovetails for measuring.


----------



## jocat54 (Mar 26, 2017)

I use drill bits--close enough for most work I do.


----------



## jlsmithseven (Mar 26, 2017)

ddickey said:


> Couldn't you use two different sizes and use the average in your calculation?



That seems like it might work, thanks for the suggestion. So say I used a .3995 and a .3985 pins (just an example of course). I would just calculate them as a .3980 pin on each side?


----------



## jlsmithseven (Mar 26, 2017)

Here is my real life example...I need a 1.771 length right. I was planning on using a .2555 and a .2455 gauge pins. I calculated my measurement between calipers for these pins as 1.08798" using a .250 measurement in my calculations. Will this work out OK? I have a .005 tolerance. Thanks guys, any answers before tomorrow would be very helpful because I plan on tackling this first thing in the morning!!!


----------



## Bob Korves (Mar 26, 2017)

jlsmithseven said:


> Here is my real life example...I need a 1.771 length right. I was planning on using a .2555 and a .2455 gauge pins. I calculated my measurement between calipers for these pins as 1.08798" using a .250 measurement in my calculations. Will this work out OK? I have a .005 tolerance. Thanks guys, any answers before tomorrow would be very helpful because I plan on tackling this first thing in the morning!!!


What exactly are you measuring at 1.771"?


----------



## 4GSR (Mar 26, 2017)

When I go to measure the location of a dovetail slot.  I generally have a sample to take my measurements from using a couple of harden & ground dowel pins of the same diameter.  You know, within 0.0005" of each other.  If I'm doing something from scratch on a drawing in cad, I generally drop in a couple of circles of a known diameter that represent the dowel pins being used.  What ever the cad drawing produces for a dimension, that is what I use to machine the dovetail to.  It's ok to show the 1.771" as a reference dimension.  I'm just trying to help here.

Your point dimension of 1.771" is impossible in the real world to measure.  A 3D laser would be about the only way to measure such a dimension.  Oh, the dovetail cutter you use will have a radius on the corner.  It may only be R0.001" but its there.  Probably turns into a R0.005" once the dovetail cutter is broken in, or much worse.  I've knocked off the sharp corners of a dovetail mills to something like R0.030", more than once, too!    My new dovetail cutters use a insert that has a R.015" or R.032" on them.  They sure help by not creating a stress riser in the sharp corners if the part is going to heat treat afterwards. 

But to go back to your question about using two pins of different diameters, no problem as long as you don't change sides the pins are referencing from.  Especially if your checking from the side of the tool block to the gage pin.  I assume you have a reference tool holder to get your pin measurements from rather than trying to calculate them.   The older Machinerys Handbooks have some good information on calculating measurements, lots of trig involved.  So much easier to lay out in cad today!


----------



## Bob Korves (Mar 26, 2017)

I have not done this particular job yet, but I would rough in my first block. making the depth cut dimension (still without the dovetails) slightly smaller to the flat than a factory holder, then machine the dovetails, very little at a time when close to size until it just fits the tool post.  Use the tool post as a gage. When they will slide together you want the depth dimension and the gage pin to gage pin dimension to match the factory part.  Go VERY slowly until you get a fit that you really like.  It should be very similar to the factory holder measurements.  Install first the factory holder and then your prototype holder on the tool post and tighten them down solidly.  The closer handle should stop in the same clock position for both holders.  If not, something is wrong.  You especially do not want to see the handle swing farther with your prototype block, that would show a too loose fit.  If that happens, make a second prototype to tighter dimensions until it closely matches the factory holder closed handle position.  Then make a bunch more just like that one, using the same gage pin and depth measurements of your successful prototype.


----------



## mikey (Mar 27, 2017)

I'd like to suggest something, may or may not be useful. Look for a *straight* rod around the shop that is 1/4" in diameter; this will hopefully be large enough to stick out of the dovetails so you can measure between them. You only need two so you can cut something in half and deburr the ends and they only need to be long enough to lodge into the dovetails ... say, maybe 1" or so. Maybe a drill blank?

We know that the base of the dovetail is 1.771" long and the angle of the dovetail is 60 degrees. The constant for a 1/4" rod at 60 degrees is 1.1830" so if you can find that rod and use it, the distance between them should be 1.771 - 1.1830 = 0.588". 

I mention this because it is fairly easy to find something that is a consistent 1/4" OD, straight and can be cut in two - printer rod or a drill blank or something like that. It is also useful because most table of constants will be based on a known diameter. 

Hope this helps. I'm attaching a pdf file that might be useful for your review.


----------



## Billh50 (Mar 27, 2017)

you can also use 2 dowel pins if you don't have gage pins. When drawing dovetails I always give dimensions using standard size pins. A couple tenths will not make a difference for most applications.


----------



## jlsmithseven (Mar 27, 2017)

mikey said:


> The constant for a 1/4" rod at 60 degrees is 1.1830" so if you can find that rod and use it, the distance between them should be 1.771 - 1.1830 = 0.588".


where did you get these numbers from?


----------



## jlsmithseven (Mar 27, 2017)

Bob Korves said:


> What exactly are you measuring at 1.771"?


The dovetail width is the overall dimension I need to meet.


----------



## Billh50 (Mar 27, 2017)

Dovetails are usually dimensioned with rolls. The overall should fall in if the dimension between the rolls is met. The reason the rolls are used is because it is almost impossible to measure into the corners of the dovetail accurately.


----------



## ewkearns (Mar 27, 2017)

The dimension for the .375 rods makes sense. The .250 rod dimensions are nonsensical, because they aren't tangent to the dovetail sides.....


----------



## Billh50 (Mar 27, 2017)

your right...I overlooked that and will fix it now


----------



## Billh50 (Mar 27, 2017)

Here is the correction.


----------



## Technical Ted (Mar 27, 2017)

What tolerance do you need to hold? Maybe someone else suggested this and I missed it, but if it were me, I'd machine a bar for the diameter you want and cut it up into two pieces of the desired length... Unless you lathe has a bad taper to it, the two pieces should end up close to the same diameter. If you have a taper, polish/file until the bar is true before cutting the pieces to length. As long as they are both the same diameter, you should be able to calculate the rest.

Just a thought,
Ted


----------



## Doubleeboy (Mar 27, 2017)

In post #1 the drawing dimensions tolerances are screwy IMO.   + - .005" for the dovetail width is going to leave you with pretty small chance for success.  It has been my experience doing dovetails on both a mill and shaper that you need to hit +- .001 for the width dimension of dovetail unless you want your dovetail to be very sloopy.  Once you have done a couple dovetails I think you will find you want to sneak up on your final dimension and try to take cuts of less than a thou at a time if you want a tight sliding fit.  One thou difference can take you from just too tight to noticeably loose in my experience.


----------



## Bob Korves (Mar 27, 2017)

Doubleeboy said:


> In post #1 the drawing dimensions tolerances are screwy IMO.   + - .005" for the dovetail width is going to leave you with pretty small chance for success.  It has been my experience doing dovetails on both a mill and shaper that you need to hit +- .001 for the width dimension of dovetail unless you want your dovetail to be very sloopy.  Once you have done a couple dovetails I think you will find you want to sneak up on your final dimension and try to take cuts of less than a thou at a time if you want a tight sliding fit.  One thou difference can take you from just too tight to noticeably loose in my experience.


+1 on the tolerance for the dovetails.  That is a precision dimension, not to be taken lightly unless you have a good use for scrap metal tool holders...


----------



## jlsmithseven (Mar 27, 2017)

I measured between a finished vice jaw and got the measurement I needed...


----------



## jlsmithseven (Mar 27, 2017)

Bob Korves said:


> +1 on the tolerance for the dovetails.  That is a precision dimension, not to be taken lightly unless you have a good use for scrap metal tool holders...



Thanks for these tips. Honestly this is just a project. We make our own and then we have to donate one to the shop. But I will creep up on the ends, just like I did in threading. Thanks for that tip.


----------



## 4GSR (Mar 27, 2017)

jlsmithseven said:


> I chickened out and just squared my other piece and milled the slot out. I am going to wait until others start their dovetails to see if I can learn from them as well. I already have everything programmed on the Prototrak so it won't take me that long to mill the other stuff out. Thanks for all the help!
> 
> When I went in this morning I wanted to tackle it, but my better judgment told me to wait. I did however find 2 pins that were exactly .250. I measured between a finished vice jaw and got the measurement I needed for my own so I'm 100% sure my method will work.


Hey, smart move.  Let the others make their mistakes and benefit from them, so when it's your turn, you will get it right the first time.


----------



## jlsmithseven (Mar 27, 2017)

4gsr said:


> Hey, smart move.  Let the others make their mistakes and benefit from them, so when it's your turn, you will get it right the first time.



It's what has happened to me this year


----------



## jlsmithseven (Mar 29, 2017)

My calculations were like .015 off, I actually went to .182 about instead of the .1955 I originally calculated. Anyways, it measures almost perfectly at 1.087 which is what I needed.


----------



## jlsmithseven (Mar 29, 2017)

Don't want to keep you guys in suspense...so in the mean time here's a spring-loaded tap center project I just completed....


----------



## 4GSR (Mar 29, 2017)

jlsmithseven said:


> Don't want to keep you guys in suspense...so in the mean time here's a spring-loaded tap center project I just completed....


Got to make one!  The P.O.S. one I bought from Little Machine Shop has over a 1//32" runout in it.
Thanks for posting.

Ken


----------



## brino (Mar 30, 2017)

4gsr said:


> Oh, the dovetail cutter you use will have a radius on the corner. It may only be R0.001" but its there. Probably turns into a R0.005" once the dovetail cutter is broken in, or much worse. I've knocked off the sharp corners of a dovetail mills to something like R0.030", more than once, too!



Hi Ken,
I have a project that requires some dovetails (also lathe tool holders).

The dovetails cutters I found have extremely sharp points(see below).
R0.001"? .......yeah maybe, it's tiny.
The project can stand a fairly large radius, as the existing tool holders have perhaps > 30 thou.(estimated with calipers)
I have an assortment of bench grinders, but NOT any kind of tool and cutter grinder.
Would you advise trying to grind a radius on the sharp dovetail points?
If so, then how?

The points look very fragile, and I'd rather lop them off in a controlled manner then have them snap off uncontrolled.

Thanks!
-brino


----------



## Bob Korves (Mar 30, 2017)

I think I would spin them against a grinding wheel, wheel face parallel to the shank, in a fixture, until you get a more robust corner, and then relieve the flats (manually with a stone if necessary) so they will cut correctly.


----------



## 4GSR (Mar 30, 2017)

brino said:


> Hi Ken,
> I have a project that requires some dovetails (also lathe tool holders).
> 
> The dovetails cutters I found have extremely sharp points(see below).
> ...


Brino,

The last cutters I sharpen with the sharp corners knocked off (dull), I set them up on my T & C grinder and kiss the corners at about 45 deg. flat about .030" to .045" wide according on the dovetail cutter size.  This so much easier than setting up my radius grinding attachment and trying to put a radius on the end.  Ken


----------



## Bob Korves (Mar 30, 2017)

4gsr said:


> Brino,
> 
> The last cutters I sharpen with the sharp corners knocked off (dull), I set them up on my T & C grinder and kiss the corners at about 45 deg. flat about .030" to .045" wide according on the dovetail cutter size.  This so much easier than setting up my radius grinding attachment and trying to put a radius on the end.  Ken


First you need a tool and cutter grinder...


----------



## 4GSR (Mar 31, 2017)

Bob Korves said:


> First you need a tool and cutter grinder...


Brino,

Your more than welcome to come down to South Texas and borrow mine!  Bring money, you could go home with one, too!

Ken


----------



## brino (Mar 31, 2017)

4gsr said:


> Your more than welcome to come down to South Texas and borrow mine! Bring money, you could go home with one, too! Ken



With another 10cm (4in) of snow predicted for today, I could really use a break from the weather!
-brino


----------



## jlsmithseven (Mar 31, 2017)

Both 100% to specs.


----------



## brino (Mar 31, 2017)

jlsmithseven said:


> Both 100% to specs.



Excellent!
Well done Justin. 

It's great to see you succeed. People here can assist, but it is your commitment to doing your best that gets it done right.
Keep it up! 

By the way, great thread you started.
I enjoyed it and learned too.

Thanks,
-brino


----------



## 4GSR (Mar 31, 2017)

Justin,

You have me wanting to build some!  

Nice job!

Ken


----------



## jamby (Mar 31, 2017)

I don't have a t/c grinder so if I need a corner relieved I just stone them back to .015 or so.   Only to keep them from breaking.

Jim


----------



## jlsmithseven (Mar 31, 2017)

Thanks for the kind words. I actually have a floppy disk I can put right into the prototrak and it can mill me out one. I was thinking of making a few more, that way I can have one for each lathe tool I use and I'll never need to waste time setting the center again..


----------



## jlsmithseven (Apr 1, 2017)

4gsr said:


> Justin,
> 
> You have me wanting to build some!
> 
> ...



You got the print, go for it! LOL.


----------



## aliva (Apr 1, 2017)

Use 2  1/4" end mills for your measuring pins


----------



## jlsmithseven (Apr 1, 2017)

aliva said:


> Use 2  1/4" end mills for your measuring pins


My teacher told me this. It makes sense. Thank you!


----------



## mccolld1 (Apr 1, 2017)

jamby said:


> I don't have a t/c grinder so if I need a corner relieved I just stone them back to .015 or so.   Only to keep them from breaking.
> 
> Jim


I made an attachment to mount my Dremel tool (nut welded the end of a holder).  Mount it in my BXA and grind the corners with the cutter mounted in the spindle of the lathe. 

Sent from my SAMSUNG-SM-G530A using Tapatalk


----------



## StuNY (Apr 1, 2017)

Thanks for the thread and all the posts guys! Would have never occurred to me to make one of these tool holders if I hadn't seen it. I made a dove tail cutter with an insert I already had and then finished my first tool holder today. I found it helpful to make the dove tail first on the back of a piece of scrap metal, tweak the dimensions based on the fit in my tool post, then make another with final dimensions to verify. Worked well, and have a nice tight fit- better than some of the cheapie ones I bought earlier. Now onto mass production mode- I always wished to have a holder for each tool!


----------



## jlsmithseven (Apr 1, 2017)

StuNY said:


> Thanks for the thread and all the posts guys! Would have never occurred to me to make one of these tool holders if I hadn't seen it. I made a dove tail cutter with an insert I already had and then finished my first tool holder today. I found it helpful to make the dove tail first on the back of a piece of scrap metal, tweak the dimensions based on the fit in my tool post, then make another with final dimensions to verify. Worked well, and have a nice tight fit- better than some of the cheapie ones I bought earlier. Now onto mass production mode- I always wished to have a holder for each tool!



LOL I'd do this too, but no room in the shop!


----------



## Rustrp (Apr 1, 2017)

Were you supposed to check the drawing for errors? The thread and pitch was correct as much as I could see, but the 3/8-24 2-A was entered UNC.


----------



## 4GSR (Apr 2, 2017)

Let's not nit pick his drawing too much, he's learning.  

Along with the UNC instead of UNF for fine threads.  The class of fit for the thread is not correct.  The 2-A should be "2B" for internal vee threads and "2A" for external vee threads.  

Ken


----------



## Rustrp (Apr 2, 2017)

4gsr said:


> Let's not nit pick his drawing too much, he's learning.


I got the distinct impression the drawing was from the school lesson plan and their instruction, along with the possibility someone would see 3/8 and UNC, then drill and tap them all the same. I did look at the print before commenting and the designer's initials didn't match, which were RCS and the print was dated 11/07/07.


----------



## Rustrp (Apr 2, 2017)

4gsr said:


> The 2-A should be "2B" for internal vee threads and "2A" for external vee threads.


True.

I also asked the question about the errors on the print because it's possible this was part of the lesson on the written exam.


----------



## jlsmithseven (Apr 3, 2017)

Rustrp said:


> Were you supposed to check the drawing for errors? The thread and pitch was correct as much as I could see, but the 3/8-24 2-A was entered UNC.


This is just from the Instructor changing it every year. He makes small changes so the 2nd years just don't give us their projects they already did....so a few things were a bit off.


----------



## Rustrp (Apr 4, 2017)

jlsmithseven said:


> He makes small changes so the 2nd years just don't give us their projects they already did....so a few things were a bit off.


I understand why he would make changes, but are you saying he makes intentional errors on the print as part of your exam? Are you required to check the print for accuracy?


----------



## jlsmithseven (Apr 4, 2017)

They're not intentional, they're careless mistakes lol. We are required to use common sense on errors, but if anything seems off I usually just ask him. Since 3/8" -24 is only a fine thread, obviously it's not UNC..right? Not trying to act like a smart-aleck....


----------



## Rustrp (Apr 4, 2017)

jlsmithseven said:


> They're not intentional, they're careless mistakes lol. We are required to use common sense on errors, but if anything seems off I usually just ask him. Since 3/8" -24 is only a fine thread, obviously it's not UNC..right? Not trying to act like a smart-aleck....


I asked the question because I was wondering if the errors were part of the exam. I'm not a fan of tests based on trick questions or ambiguity, although some instructors do practice it. If you have advanced to cutting dovetails, misleading drawings waste time unless it's part of every project. Since the UNC was incorrect along with the thread fit class being incorrect, which Ken pointed out, and I was just asking. With that said, it seems they would have someone check the drawings and note revisions, date them and who checked the Dwg. -Russ


----------



## ewkearns (Apr 5, 2017)

brino said:


> Would you advise trying to grind a radius on the sharp dovetail points?



1) Absolutely no reason to fiddle with a radius....


----------

