Tolerance for Dowel Holes

[Speedy]

I want to specify a press fit dowel hole for an M20 dowel.

I always understood that all dowel holes were drilled and reamed to class H7, i.e +0.021 -0.0 mm on DIA 20.00

I see that there are 2 types of dowels, h6 and m6.
Values on dowel would be
h6 = +0.0 -0.030mm for M20
m6 = +0.008 +0.021mm for M20

My question is do I simply use the m6 to give the interference on the H7 hole, or do I alter the hole for the standard h6 dowel?

Am I right in assuming that h6 is the more standard dowel?
Most dowels I used before on H7 holes were always tight but not press fit.

Speedy

 

[israelkk]

If you look on the tolerances you can see that even the m6 can have a loose fit. For example if the actual dimameter of the m6 pin is 20.008 and the rimmed hole is 20.021 than there will be no press fit at all.

 

[eromlignod]

Unless you're wanting a fit for a critical application, or you are working with some sort of anal-retentive government spec., you can get way too scientific (and expensive) about a force fit.

You have to look at it from the perspective of the machinist. What do you think he's going to do when he sees your tolerance? He only has so many options. He can give you any tolerance you want by laboriously boring, honing, lapping, shell-reaming, etc., but in reality, for an ordinary dowel press-fit, you and I know he's just going to grab an undersized reamer and ream it.

It took me several years as a young engineer to realize that my exotic specifications were the source of much amusement in the machine shop.

While specifying meticulously thought-out limits might be more scientifically sound, it also wastes a lot of your time and the machinist's time. Anymore, unless it is a critical application, I just give the hole its nominal dimension and add a note to press fit it to the dowel that's specified in the BOM. That way he can measure the actual pin, pick a reamer and be done with it.

Don
Kansas City

 

[handleman]

If you want to ensure an interference fit with a standard H7 hole you can order dowels with a p6 tolerance.

p6 = +0.022 +0.035 for M20.

These are available from Misumi in 50, 60, 70, and 80mm lengths (with an M10 tap in the end for removal) for USD $1.40 each.

I'm not certain for such a large hole size, but I'm pretty sure that changing from the H7 on your holes will increase the machining cost for the part.

 

[Philrock]

You also need to consider 2 other things:

1. How is the joint being loaded? If you have heavy reversing loads, you should have a press fit. If you have only light loads, and precise positioning is not critical, a loose fit is o.k.

2. How many dowel pins are in the joint? If there is more than one, holes will have to be match-machined, or machined at super tight tolerances in terms of location, in order to get them to line up for assembly.

 

[israelkk]

handleman

First, even with the p6 in a worst case scenario the interference may be only 0.001mm which may be insufficient if the pin sees high side loads.

Secondly, specifying H7 or even H6 on the hole does not increase the machining cost because the hole can be reammed which is a simple process similar to drilling.

 

[handleman]

I may have been unclear in my wording. I was intending to say that if you use a hole tolerance OTHER than H7 (like K7) you may increase your cost. This depends a lot on who is making the part and how many they are making. If your shop has to buy/modify a giant undersized reamer or jig bore one hole you will certainly increase cost much more than buying a p6 pin.

 

[Speedy]

Thanks for all your replies.

In this application the dowel will more than likely be 'fried' over time and will have to be replaced at regular intervals. The environment is in a high pressure combustion chamber with extremely high temperature and pressures.

The reason for all the fuss over the hole tolerance is that I don't want the customer to have to go running around looking for non-standard, difficult to get dowels.

So to put the question simply;

What is the tolernace class on a 'standard' dowel?

Cheers,
Speedy

 

[Tunalover]

eromlignod-
So you are advocating just telling the machinist to install the pin with a press fit? What's a press-fit?

Machinist 'A' gives one that's just shy of a running fit; he argues that he's unable to pull the pin out with all the pull he can muster with his fingers. He calls this a press-fit. Of course the minute the part sees a temperature extreme or gets a jolt in service the pin pops out (if it doesn't interfere in the assy).

Machinist 'B' gives a press-fit that is very tight and results in the scrapping of one host plate and six pins before he gets it to his satisfaction.

Machinist 'C' has thirty years in the business. Because so many of his (lazy, cavalier,...) customers have specified only "press-fit" over the years, he uses a mental formula he has accumulated over the years that depends on the materials, installation depth, and size. He knows what holes to create in the plate based on empirical experience.

We would all choose 'C' but how many machinists are out there that meet this description?

Which Machinist would you choose? When was the last time you saw a machinist's resume from your fabricated metalwork supplier?

The only low-risk approach is to specify the fit with hard data such as that from a long-published, high-confidence source such as Machinery's Handbook. If the data's cannot be found then I'd be inclined to do some experimentation before cutting a PO for thousands of dollars worth of parts!

The devil's in the details. It's the engineer's job to walk a fine line between the supplier's due diligence and being "overly-detailed" with the drawings. I tend to favor the latter if the part's failure jeopardizes safety or incurs substantial financial loss on behalf of my employer or his customer! Now I get off my soap box.



Tunalover

 

[eromlignod]

If you'll read my post again you'll see that I was referring to a non-critical application. The practice of calling out a press fit as "PF" on a drawing is common and widespread and has been in use since long before my 21 years in industry.

Most of the time in machine design, dowels are used as locators so that a part can be removed and will retain its accurate location when it is replaced. They are usually designed to press fit into one part and locationally fit into the mating part, simply to retain pin so that it doesn't get lost. There is nothing critical about the force fit in this extremely common application.

Don
Kansas City

 

[KENAT]

I've seen all kinds of things specified on drawings along the lines of:

"Hammer to shape, file to fit, and paint to match"

In my opinion that doesn't necessarily make it good practice, perhaps just a common bad practice.

You say the dowels will need to be replaced, is relying on interference fit a good idea in this case. Over time is the hole not likely to grow as you repeatedly remove & install dowels?

As regards customer supplied dowels, I'd suggest that in the maintenance manual you need to state the required dowel tolerance. You could design the hole around 'standard dowels' but it is quite possible the customer will end up with a 'non standard' dowel. I'd design the hole for a dowel that is relatively easy to obtain but still specify the required tolerance, or perhaps even the supplier part number, in the manual.

Of course you could be really financially astute & assign a Part Number to the dowel so that the customer has to order dowels from your company every time he wants/needs to replace one!

 

[ccfoam]

Good Afternoon

I've learned a few things about dowels in my 25 years of Tool Engineering concerning dowel pins.
1. NEVER use dowels to resist forces, NEVER.
2. NEVER press fit a dowel pin into a blind hole, because you can't pull them out, you need to knock it out.
3. Press fit the dowel into the part that is not consumable because once the hole wears from multiple press fits, the location is gone.
4. Slip fit the dowel into the part that is a wear item so that when the dowel holes become worn, you replace the part.
5. NEVER use dowel pins to resist forces, NEVER.

 

[dimjim]

Will a spring pin work or do you need the
strength of a solid pin?

 

[handleman]

2. NEVER press fit a dowel pin into a blind hole, because you can't pull them out, you need to knock it out.

That's why they make dowels with tapped holes in them, as per my first post. Slightly more expensive, but in machine design sometimes it's better to use a more expensive cheap part than to make an expensive part more so.

 

[Tunalover]

Speedy-
Yesterday I specified a press-fit dowel pin for a part I designed. Look in Machinery's Handbook under "fits" or "cylindrical fit". ANSI B4.1 (if I recall correctly) specifies different cylindrical fits depending on the application. I called out a "CLASS LN2 FIT PER ANSI B4.1 FOR A .0625 NOMINAL DIAMETER SHAFT" for an MS16555-601 dowel pin (1/16" nominal dia stainless steel dowel pin 3/16" long per NASM16555). I was looking to closely control the pin location so I chose an LN fit class (there are three).



Tunalover