# Countersink a hole to a specific dia. help



## jlsmithseven (Oct 8, 2017)

Hi guys,

Something I've struggled with since last year has returned. I use it at work all of the time, but for some reason the formula doesn't want to stick with me.

Say I drill a hole with a 3/8" drill and the print calls out for a .425 diameter hole chamfer on it. I understand I need to use a 1/2" countersink, but I struggle with grasping how deep I need to go on the hole.

I also understand how 82,90, 118 included angles all make a difference in the calculation. I know that 90 degrees is the easiest to figure out because you divide it by 2, but then I get lost again. I've had many people explain it to me, but I was wondering if any of you had a quick and easy method to make it stick. I appreciate your help!

*82 and 90 deg. are about 99% of what I do so if you could explain both of those it'd be awesome.*


----------



## higgite (Oct 8, 2017)

If you are near a computer when you need the info, or if you have a smart phone with a browser, try this:
http://janproducts.com/CounterSink_Calculator.html

Tom


----------



## jlsmithseven (Oct 8, 2017)

I have seen that website, but it doesn't help me much.


----------



## woodchucker (Oct 8, 2017)

jlsmithseven said:


> I have seen that website, but it doesn't help me much.


The calc Seems to work for me.
.425  82degree = .2445 depth.

edit, it appears to be correct. I tested using a 118, then realized my mistake.
just checked with an 82 degree chamfer bit.


----------



## RJSakowski (Oct 8, 2017)

The depth of the countersink, as measured from  the tip of the countersink is x = d/2*cot( A/2) = (d/2)/tan(A/2) where A is the angle of the countersink and d is the diameter of the countersink. Scientific calculators  are available on most, if not all, computer operating systems and on Android systems. For an 82º countersink, cot(82/2)= cot(41) =1.1504.  For a 90º countersink, cot(90/2) = cot(45) =1.

This assumes a sharp point on the countersink.


----------



## Wreck™Wreck (Oct 8, 2017)

Bloody hell pull the other one, a 90 Deg. chamfer is 45 per side or the diagonal of a square, one does not require trig to figure this out, other angles are no more difficult. Measuring such a feature however is a different matter, the math is simple and straightforward. In practice your machine will have errors. A countersink gauge is one method yet I suspect that you will not likely want to spend $300.00 for one tool with a specific purpose. I could be wrong.
https://www.mscdirect.com/product/details/86445178


----------



## 4GSR (Oct 8, 2017)

When ever I need to countersink a hole for a flat head screw, I use the screw for a gage.  
I've never in my life has a specification for a countersunk hole to be held to a specific diameter any tighter than +/-.03".  Which most of the time, I eyeball and move on to the next hole.  And if someone gives me flack over it, I'll pull out my cordless drill, put a countersink in the drill, give it to them and say here you go, fix it your way!


----------



## markba633csi (Oct 8, 2017)

I got the same result with the online calculator: 82 deg  and .425 = .2445 depth
But I always use a screw as a gauge.  Too lazy to do the math. 
Mark


----------



## T Bredehoft (Oct 8, 2017)

Use a screw, but you'll quickly find out the screw head isn't the diameter of the c;sunk cavity. Ya gotta go deeper.


----------



## Franko (Oct 8, 2017)

I would probably put a scrap piece in and nibble at it until it was correct, using the bolt head as a guage. Record how deep the plunge was and use that on the finished piece. I would zero the plunge from where the countersink makes contact with the starting hole.


----------



## higgite (Oct 8, 2017)

I have only done a couple of countersinks, but here is how I avoided all the math. I’m open to better methods.

Once you have your hole drilled or threaded, drop or thread your screw into the hole as far as it will go. Then lower the spindle to touch your countersink bit to the flat part of the top of the screw and zero the Z-axis readout. Then move over and touch the bit to the top of the work piece. Note the reading. Remove the screw from the hole and realign the bit directly over the hole. Now lower the bit until it touches the rim of the hole. The point of the bit will be below the work surface. Hold it there and zero the Z-axis readout. Now drill the countersink until the Z-axis readout matches what you noted earlier. The screw should now fit flush with the work surface.

Tom


----------



## tq60 (Oct 8, 2017)

If you want it clean you need a bit the same as the OD of the screw so you can counter bore the thickness of the top of the head if it has any meat on it.

We made a tool to countersink screw holes in the wood to of radial arm saw where we wanted the screws a bit under the top to insure no possible scratching.

Having the counter bore just looks better as it is a bit difficult to get the depth perfect.

Too deep with wider tool and you have a ring around the head and too shallow the head protrudes.

Counterbores avoid the ring and once the first one is depth stopped the rest are easy.


Sent from my SAMSUNG-SGH-I337Z using Tapatalk


----------



## RJSakowski (Oct 9, 2017)

Wreck™Wreck said:


> Bloody hell pull the other one, a 90 Deg. chamfer is 45 per side or the diagonal of a square, one does not require trig to figure this out, other angles are no more difficult.


I believe the OP asked how do you calculate the depth of the countersink, given the major diameter and c'snk angle. 

When we sent out drawings for machining we specified the major diameter and angle.  That was the only practical and unambiguous way to specify that feature.  It was up to the machinist to figure out how deep to go to achieve the spec.

For my own work, I will use a trial and error method as has been suggested by others.  I have the specific fastener at hand and can set my parameters to achieve the fit that I want.  Not so for someone working from a drawing.


----------



## Wreck™Wreck (Oct 9, 2017)

For an 82 1/2  deg. counter sink the diameter X .571 is more then close enough.

.243 from the theoretical sharp point.

If in your case you touch the countersink off on the .375 hole edge the difference in diameters X .571 will yield the depth.

.425 - .375= .05
.05 X .571= .0285 depth which will be more then close enough for such work, the countersink itself will have a +- 2 Deg. tolerance or so.

A 90 Deg. countersink is of course.500 because it is a right triangle.


----------



## jlsmithseven (Oct 11, 2017)

Thanks for the input. So I get the calculator now. But does this matter no matter the size of the countersink. Say I calculate .250 I need to go down, it doesn't matter if I use a 1/2 or 3/4 diameter countersink , I will always go that deep to reach the required diameter. Because thats what it asks for, diameter and included angle. Am I correct ?


----------



## woodchucker (Oct 11, 2017)

its all about the angle, not the diameter of the bit.


----------



## Tony Wells (Oct 11, 2017)

Larger countersinks often are not sharp pointed, but flat, so you have to work off where they contact the existing drilled hole. Then comes a little math if you have a spec to meet, or a sample screw, which btw does not have a sharp edge at the top, so if you just measure the screw and cs to that, it will sit proud. You'll have to go deeper to get flush.


----------



## Wreck™Wreck (Oct 11, 2017)

jlsmithseven said:


> Thanks for the input. So I get the calculator now. But does this matter no matter the size of the countersink. Say I calculate .250 I need to go down, it doesn't matter if I use a 1/2 or 3/4 diameter countersink , I will always go that deep to reach the required diameter. Because thats what it asks for, diameter and included angle. Am I correct ?


Yes, the angle remains constant regardless of tool diameter.
As Tony Wells mentioned, finding the theoretical sharp point of a countersink is problematic, few such tools have sharp points. In the graphic representation shown below if you were to touch off the countersink at the sharp edge of the .375 hole then advance .029" in you would achieve your .425 diameter in a perfect world, we do not live in a perfect world however, any error in the tool, machine spindle and your ability to pick up a sharp edge will effect the finished size. The ratio .571 works for this angle only.

Included angle is both sides combined, in round (lathe) work excluding threading this is almost always true, a 60 Deg. V thread is two 30 Deg. angles in relation to one axis plane. A buttress thread may have an included angle of 50 Degrees, one being 45 and the other being 5


----------



## jlsmithseven (Oct 12, 2017)

Thanks guys I believe I understand it now. The calculator will really help me, but I have a better understanding of what needs to happen.


----------



## Billh50 (Oct 12, 2017)

I just go deep enough that the head of the screw is .005 - .010 below the surface. That way any difference in other screws will still be below the surface. except when countersinking sheet metal then I just go deep enough the screw feels flush.


----------



## jlsmithseven (Oct 14, 2017)

Good news, the countersink calculator works great. My diameter was perfect.


----------



## jlsmithseven (Oct 16, 2017)

So here is my first real Haas Lathe CNC Project all completed. The countersink depth is perfect and I used a spot drill to get to that measurement. Pretty cool.


----------



## Wreck™Wreck (Oct 16, 2017)

What is the material?


----------



## jlsmithseven (Oct 16, 2017)

CRS 1018, why do you ask?

Edit - This is actually the part I scrapped. I made a few minor changes to the RPM's and facing (because it didn't face on this part).


----------



## jlsmithseven (Oct 21, 2017)

Speeds + Feeds make all the difference in the world. Faster RPM's spinning gave me this shiny part. MUCH better product.


----------



## Wreck™Wreck (Oct 23, 2017)

jlsmithseven said:


> CRS 1018, why do you ask?
> 
> Edit - This is actually the part I scrapped. I made a few minor changes to the RPM's and facing (because it didn't face on this part).


I ask because in the future your employer will give you a drawing and say make 30 of these by Wed.
The first question that you should ask is, what is the material and in what condition is it.

A drawing may specify CRS 3" round material, this gives you little information to work with, one material in a particular condition may turn easily, the same general material in a different condition may take far longer for the same part.

I see that you have discovered the fact that the faster you turn it the better the finish, well done


----------

