Questions on Milling Dovetails

Hello,

I'm new to machining dovetails and looking for some information. Specifically, I'm interested in machining O-Ring dovetails similar to the ones attached (Both trapezoid cross-sections and ones with a flat vertical wall). What do I need to watch out for? What are good references for feeds & speeds? Chip loads? Do you cut both sides of the angled walls at the same time? What are the pros & cons of using a solid tool vs. a tool with inserts (Tolerance? Cost? Repeatability? etc). I'm cutting standard metallic materials such as Aluminum or Steel. I know these can be turned as well, but right now I'm looking for milling on 3, 4 or 5 axis mills.

I believe you usually cut the rectangular portion of the slot with a standard mill and then go back with the dovetail mill - are there rules of thumb for this? (Cut depth to the slot bottom? Over / under slot bottom by a couple thousands of an inch? etc.) Is the standard mill the same size as the pocket? under sized?

Thanks in advance for any assistance.

mtags said:

Hello,

I'm new to machining dovetails and looking for some information. Specifically, I'm interested in machining O-Ring dovetails similar to the ones attached (Both trapezoid cross-sections and ones with a flat vertical wall). What do I need to watch out for? What are good references for feeds & speeds? Chip loads? Do you cut both sides of the angled walls at the same time? What are the pros & cons of using a solid tool vs. a tool with inserts (Tolerance? Cost? Repeatability? etc). I'm cutting standard metallic materials such as Aluminum or Steel. I know these can be turned as well, but right now I'm looking for milling on 3, 4 or 5 axis mills.

I believe you usually cut the rectangular portion of the slot with a standard mill and then go back with the dovetail mill - are there rules of thumb for this? (Cut depth to the slot bottom? Over / under slot bottom by a couple thousands of an inch? etc.) Is the standard mill the same size as the pocket? under sized?

Click to expand...

Chips, chip control is the challenge (when Milling) Rough as much out as you can before you try generating a feature. A GO/NOGO is supremely helpful with Dovetail Grooves (when Milling).

If those are OD Grooves on a round part....Milling them is just an insult. Turning would make a hardish question about "how to", into a piece of cake with no real questions involved. To be honest, if you have a Lathe that will do it, and you don't do it that way, sheesh, you got a long road ahead of you.

R

Any help ?

Harvey Tool - Carbide Dovetail Cutters - Parker Hannifin O-Ring Dovetail Cutters WITH Drop Hole Provision

And Harvey Tool - Carbide Dovetail Cutters - Parker Hannifin O-Ring Dovetail Cutters WITHOUT Drop Hole Provision

litlerob1 said:

If those are OD Grooves on a round part....Milling them is just an insult. Turning would make a hardish question about "how to", into a piece of cake with no real questions involved. To be honest, if you have a Lathe that will do it, and you don't do it that way, sheesh, you got a long road ahead of you.

R

Click to expand...

They're not - I should have clarified. "I know these can be turned in some instances but the feature is either not turnable, or the part is to large to making turning practical."

Any insight to the pros / cons of tools with inserts vs. not? Why would you pick one over the other for dovetails?

If the two configurations are dimensionally similar, then the lower one would likely accommodate a more robust dovetail cutter. Another factor that you might want to take into account is how to measure your dovetail.

P.S. Use of o-rings usually implies a desire to seal a specific volume. If this is the case you might also want to consider a strategy for entering and exiting the cut that doesn't impair sealing capability. (e.g. entering and exiting within the area to be sealed.)

The first straight cut thro the center is known as the "Primary" slot its normally slightly deeper than the finished depth of the dovetail if the depth is not stated on the drg make it .010 deeper to stop the dovetail rubbing and cuttings becoming trapped and breaking the tool.Its not reccomended to go thro in one cut on the dovetail a tool like the top view of your examples would be preferable as will allow superior swarf clearance it would be a pass thro the primary slot and open it up both ways untill the desired width is obtained,Theres no way that I know of doing these quick if you find a way let us know

If it's your design, give yourself a drop hole allowance if you're going to mill these grooves. If it's not on the drawing and you're not the designer, ask them about allowing it, or getting it added to the drawing. A tool that will fit through the opening at the top and still cut the dovetail geometry you want is going to tend to be extremely fragile.

If it's your design and you haven't reviewed the Parker O-ring handbook recently, take a look. You might be surprised what you can get away with for a face seal if you don't need the retention of a dovetail groove.