G10/FR 4 Plastic Material

[SpecialtyTool]

Does anyone have much experience machining G10/FR 4 plastic material? I know carbide is pretty much the only way to go but I was wondering about feeds and speeds. I basically need to first square up the material, cut some pockets with 1/8", 1/4", and 1/2" endmills. I also have to drill (15) .067" dia holes thru almost 1" of material. I have ordered some circuit board drills for them but I have no idea about feeds and speeds for anything (drills or endmills). Any help would be appreciated.

 

Thanks

[RonC.]

Try this seems to work for me

G10/G11

carbide

sfm = 200-500

feed per tooth

1/8" = .001

1/4" = .003

1/2" = .006

 

as for drill = .0003 per tooth

 

hope this Helps

Ron

[jeff]

I've cut this stuff quite a bit, and I've found that the Accupro 2 or 3 flute endmills last the longest (of the ones that I've tried).

 

TiCN coating (the darker orange coating) seems to be really good.

 

Speeds = I would go a little slower than you would in mild steel on RPM's because it's abrasive.. we have to cut it dry for our customer's specs.

 

Also make sure you approach exiting corners in such a way that it doesn't break, because it's a laminate it will tend to break on exiting.

 

Nasty stuff, gives me an instant headache whenever I smell that crap being cut.

[Thee Dragracer1951]

Uh

Brae

Siv

 

I HATE cutting that stuff

And I get to a lot...

200 or so SFM

Ron's chip loads are jsut about what I run

If you are drilling a lot of holes, use carbide drills. .063 holes, I'd be pecking about every .05 just to clear the chips

You'll likely need to ream them to size if your tol is tight

I use carbide reamers to get a little life out of them

[SpecialtyTool]

What about sawing it? Any tips? It started to break apart on us.

[jeff]

What about sawing it? Any tips? It started to break apart on us.

 

Saw it larger, that's all I got for that. /shrug

[Thee Dragracer1951]

^^^

Troof

[CADCAM3D5AXIS]

You want to make sure your making chips and not powder, if you smell it really strong your burning it not cutting it.I like to ruff within .050 on all walls and surface to keep feature details from breaking and looking like crap. and this works pretty good for me on all types of laminates that crumble on the corners. 3M has some info on there site about this and other plastics when i find my info I will be glad to share if no one gets to it before me

HTH

[CADCAM3D5AXIS]

Here is some info on a variety of materials with G10 in near the bottom.

 

http://robbjack.com/technical/speed-and-feed

 

HTH

[SpecialtyTool]

So the parts didn't work for the customer and we have to remake them. It is an issue with the small holes. Apparently they are going to have to be reamed. Im not sure if its going to be a press or slip but either way, what size reamer should I get in comparison to the hole I need? On size, over sized, or under? And by how much?

[jeff]

On size to the dimension you need to hold. MAYBE... MAYBE a couple of tenths over, but that's pushing it.

Buy more than one, especially if you go with the standard HSS reamers.

I think carbide reamers might not be cost effective, depending on the price you're able to acquire them at.

 

If money isn't an issue, you might want to try diamond coated for the added abrasive resistance.

[within a thou]

Sandvik came out with a line of Carbide drills for composites that are supposed to eliminate the burrs and chipping on break out. Call them and have them do a demo in one of the scrap parts before you buy.

 

http://www.sandvik.coromant.com/en-gb/products/corodrill_854_856/Pages/default.aspx

[jeff]

Sandvik came out with a line of Carbide drills for composites that are supposed to eliminate the burrs and chipping on break out. Call them and have them do a demo in one of the scrap parts before you buy.

 

http://www.sandvik.c...es/default.aspx

 

The only thing I know about Sandvik solid carbide drills is that they are expensive! The sales rep even told us that lol.

BUT.... these look like a good buy if they work.

[within a thou]

The only thing I know about Sandvik solid carbide drills is that they are expensive! The sales rep even told us that lol.

BUT.... these look like a good buy if they work.

 

I am unsure but I watched a demo of them in some 17-4PH 16mm or 18mm diameter feeding at 38.6ipm and it wasn't struggling. Think it was 4xD. They ran the same size drills in both their 880 (the whole drill tip is carbide) and their udrill they ran at 19ipm and 10ipr respectivly.

 

They also had a 6mm solid carbide 30XD that was running 8ipm the full depth of the flute. I wouldn't have believed it if I hadn't seen it. You need a pilot to start the drill and if you turn the high powered STC on before the drill is in the hole it will snap.

[rrReagaN]

I'm about to mill some G10 for the first time on one of our HAAS machines. This thread and a few others were helpful and hopefully put me in the right direction.

[jeff]

I'm about to mill some G10 for the first time on one of our HAAS machines. This thread and a few others were helpful and hopefully put me in the right direction.

Just be careful with outside corners, it's easy to have the laminate come apart, you may have to do some finaggelin.

[civiceg]

For sawing get a grit blade, works awesome. 

[jeff]

For sawing get a grit blade, works awesome. 

What is a grit blade?

[civiceg]

http://www.starrett.com/saws/saws-hand-tool-products/band-saw-blades/carbide-diamond/advanz-dg

 

I will get the correct one we order monday, I really don't think they are too bad cost wise and they last. I used to weld them back up and stay away from the diamond when they would break for over feeding. 

[jeff]

http://www.starrett.com/saws/saws-hand-tool-products/band-saw-blades/carbide-diamond/advanz-dg

 

I will get the correct one we order monday, I really don't think they are too bad cost wise and they last. I used to weld them back up and stay away from the diamond when they would break for over feeding. 

How much is that blade? We have a ton of G10 to saw in a vertical band saw and it's a pain to push that thru the blade.

 

seems to be about $210 for a 12foot carbide grit blade.

[civiceg]

I don't know the actual cost, I can find out Monday. But, I know its justifiable for our company because we only cut G10 with them. We have them for both our manual and automatic saws.

[civiceg]

We buy them from a local supplier, they are Lenox blades and are 300 bucks.

[Machineguy]

Just a work of caution.

This is fiberglass material. This stuff get into the air , gets on your skin, and in YOUR LUNGS!!

WEAR PROTECTIVE GEAR AT ALL TIMES. GET  A VACUMN THAT HAS A MICRO FILTRATION SYSTEM SO IT DOESN'T GET BACK INTO THE AIR. And use it.

Don't rum your skin during or after use. Wash, Wash , Wash.

 

It doesn't take much to cause a lot of problems down the road.

 

Machineguy

[civiceg]

Cold water when you wash as well.

[rrReagaN]

Just be careful with outside corners, it's easy to have the laminate come apart, you may have to do some finaggelin.

Hey jeff I'm gonna be honest and I nailed it first try. I wasn't surprised that it passed inspection but I was surprised that I had no problems at all, and was a two piece part for a bad xxxx LOX rocket engine with some moderately tight tolerances. I adjusted from the suggested info and had to use a chamfer mill and ball to mill a 0.03" fillet with no delamination on the entire part. I ran it dry with a respirator and used a shop vac. Thanks for the reply.