Machining operation (fillet) on Aluminium block

[sundeep198]

Hi all,
I have Aluminium block which is drilled from 2 sides at 90°.

Problem:
A sharp edge is created at intersection of both the operation.
Due to this there is a pressure drop. We did a CFD analysis for this.
So for this we need to add fillet/radius at the intersection zone. (on the edge)

I need to know, what is the process by which i can get the fillet at the zone.
Also need to check its feasibly for high volume parts.
Please refer the attached pdf which indicate the requirements.

regards,
Sundeep

link to file:

http://files.engineering.com/getfil...96-8d15-5f6e5b603d96&file=Aluminium_block.pdf

 

[ajack1]

I would finish the drilling off with a ball nose cutter in one direction,

 

[sundeep198]

but still the intersecting edge would be formed.

 

[ajack1]

Okay maybe I am not understanding what you are after correctly. If you are looking at putting a chamfer or radius on the inside edge where the two meet that is more of a problem.

Whilst it will not put a true radius or chamfer on have you considered abrasive flow machining? Basically it involves forcing a type of abrasive “putty” through the inside of parts to improve the surface finish / remove burrs, similar end product to “rumbling”.

 

[hydtools]

I would be surprised if that edge is causing significant flow loss compared to that caused by the 90 deg turn. It may not be worth the effort to solve. What is your fluid and flow rate?

Ted

 

[MikeHalloran]

You can probably rough out that interior fillet with a ball cutter in a CNC mill, but the cycle time will be very slow because you need a reduced shank cutter to get in there. It will require handwork to get a nice finish; in fact there may be no penalty for doing all the cutting with handheld Dremel tools.

Or go for the abrasive flow machining.

Depending on the particular aluminum alloy in use, you might be able to machine the elbow bore in a straight condition and bend the part after machining. You will probably have to use a larger bend radius than you have shown, and neck down the outside pre-bend.

If you are at a fairly early stage of development, you owe it to yourself to spend some time in a junkyard and look at how automotive air conditioning stuff is assembled from aluminum tubing with end fittings that are coined or formed or machined from extrusions, and everything crimped and brazed and then bent, etc.





Mike Halloran
Pembroke Pines, FL, USA

 

[BillPSU]

You could modify the design to change the 90 degree to a large angle if possible. You could also use oversize end fittings on the hose connections and increase the bore diameter of this 90 degree thus increasing the area slowing the fluid around the corner, reducing the pressure drop.

I would not try to change the corner inside the part. They will have a hard enough time removing the burrs in the area you are concerned about. The bending concept of MikeHalloran is also interesting.

Bill

 

[shamgarbrett]

For cross-hole deburring and interior edge radiusing, I'd recommend one of these tools:

http://www.deburringtechnologies.com/

Most are suitable to CNC cycle programming which can be done in large quantities with consistent results. There are a few other internal deburring tools out there which might work the same. Call some vendors, get them to bring samples by and help with the application.

good luck.

 

[Guest0527211403]

Also need to check its feasibly for high volume parts.

If you're going to high volumes, you may also want to look at making the entire block as an aluminum casting and machining any threads for fittings, etc afterwards.

You can achieve the internal fillets with a core fairly easily.