[wjbzone]

I am machining a part that our sales rep told us was an Aluminum composite. I assumed it would be easy to machine.

The material callout on the print is AlSiC-30%. It is a cast Aluminum-Silicone-Carbide composite.

I've burned up carbide inserts, HSS tools and drills. Tried different speeds and feeds and depths but no luck. I just keep changing inserts after every pass.

I am going to have to pass on the drilling operations.

It cuts ok at first, until you get through the rough cast outer layer.

Hope to be able to turn it. I have some diamond inserted turning tools that might work.

Can anyone give me some suggestions on machining this material?
Bill

[mxtras]

What do your cooked tools look like? Are they breaking, chipping, or are they just acting dull instantly? Sometimes it is hard to catch the real mode of failure - chipping usually comes shortly after dulling, but not always. I have seen bad batches of inserts that were probably overheated during finishing, for example.

Have you tried neutral or maybe even slightly negative rake geomtries? I think the secret is in tool geometry and cutting speed - you have played with the latter, but how about the tooling geometry? Maybe your sales rep can contact the factory and get their input?

Sorry for the questions and I am sorry I don't have experience with this same material. I have been in the same boat with composite armor plating and Ferrilium in the past - some of the hardest materials I have had to machine. By looking very closely at the tool, you can hopefully develop the solution....I call it 'analytical persistence' - AKA the 'empty wallet' syndrome.

Scott

[wjbzone]

The tools are going dull instantly. They chip if you leave them in for long.

I did try a varity of speeds, but did not use anything but positive rake tools.

I'll have a look at some different tool geometries.

Thanks,
Bill

[mxtras]

A story about tooling geometry:

In about 1988 I was working as a tool maker/grinder at a machine tool manufacturer here in Virginia which had some of the East coast's larger mills and VTLs. Because of the capacity, they would occasionally get sizeable contracts from Newport News Shipbuilding for parts too large or too numerous for NNS to handle.

One such project was the catapult rails for the USS Washington and USS Lincoln - two new Carriers they were building. The material was extremely, extremely tough and super-duper-secret. The Navy made us account for and return ALL of the chips with weight records....I guess they were pretty proud of that material.

Each rail had many, many 36MM (1.42") holes drilled through for mounting and we had hundreds of these things to run. At first, we were getting one hole per drill - the material was absulutely destroying the cutting edge. Of course, we tried a zillion different ideas then we started looking at geometry. I was tasked with keeping the machinist stocked with tools so I started playing with the geometry of the drills first.

To make a long story short, I looked very closely at the wear pattern under a scope and based on what I saw, I began playing with the included angle of the drill, analyzing the results of each change. A standard drill is 118 included, you use 135 for stainless, 100 for aluminum. A 118 drill would go in about 3/8" before it was dull. A 135 drill would go through but it was dull near the end of the drilling cycle as noted by motor load of the spindle.

I backed away from 135 in 5 degree steps and saw promise, but still unacceptable results. 120 was no good, 130 was the same, but 125 worked pretty well. After lots of playing with everything else, I ended up at 126.5 degrees. At 126.5 we could drill up to 18 holes! It boiled down to .5 degree difference - 126=one or two holes. 127= one hole. But 126.5 would drill almost half the part!

Eventually we were able to drill all the holes in each part with just one drill, but it took maybe 2 days of constant refinement - you may not have that luxury.

Anyway - one experience with altering tool geometry successfully to overcome what appeared to be an impossible task.

Scott

[firedog]

I have had some experience with MMC materials (metal matrix composite). These have high si content and have ceramic wiskers imbedded into the material. The only thing that works very well is PCD coated inserts and drills. Using standard carbide or hss will not work because the material is so abrasive. PCD is not cheap, but about hte only answer.

[mxtras]

Something doesn't sound right here - not if what wjbzone is talking about IS truley a MMC.

If so, this might be a classic case of the machinist getting the shaft for an engineers' poor decision on material or process.

MMC materials - how do I say this - you would not be doing the material justice if your design called for secondary machining operations. You would be defeating the advantages of MMC. One main advantage of MMC is the ability to cast or forge net shape or near-net parts which may require finer finishin ops than machining - such as grinding.

MMC are typically used for volume, net-shape parts - not as a raw material for machining! I know this rant doesn't help your situation, wjbzone! Sorry.

Scott

[mxtras]

What happened with your attempts, wjbzone?

Scott

[BillPSu]

This type of MMC material is typically called whisker reinforced aluminum. This material is used in application where light weight and great stiffness is required. Machining this material can be performed using poly crystalline diamond as per firedog but it can also be cut using EDM or wire EDM or grinding. I assume ECM could also be used. I personally have no experience machining this material but a friend of mine related his experience to me and I researched the material. The friend was machining parts of an inertial guidance system for a satellite or a missile.

[wjbzone]

I've been off and on this job. We made some cuts with some diamond tools that we had here. That worked better then the carbide which was useless.

I just got in some PCD tools for testing today. Got some positive, neutral and negative rake. Will be cutting this afternoon. If that goes well, I need to have a groover tool made up in PCD.

I found a local place here in Dayton that will make it. I think the groover will cost about $130 each.

Will let you know how it goes later. Thanks for the help.
Bill

[wjbzone]

We made the roughing cuts using some 80° PCD tools. Worked good. The recommended speed was 1000-2000 SFM ;0.001-0.002 ipr ; 0.025" depth.
We found it cut better at about 250 sfm and 0.005 ipr. Left a good finish. (±63).

I ordered a groover and some 55° inserts to finish the job.
Bill

(negative rake tools)