CNC Mill Reccomendation

[pauls]

The attached pic is similar to the cnc flanges we make for turbo setups. The problem is they take forever on our industrial hobbies machine. The material is 1/2" CRS. The flanges are 3" x 14" long. Currently using a 1/2" 4 flute carbide mill, cutting pockets and then contour the outside. The max the IH mill will go is .07" depth at 6ipm. Any more the machine shakes or the spindle bogs down. Can take lighter cuts but even with .02 can't get faster than 10 ipm. Its time to get a real mill. We have loads of parts to make. Can anyone give me an idea how I would cut these and approximate time to complete on an entry level Haas or equilvilant. I'm going to visit some dealers in the next month.
Thanks
Paul

Similar Threads:

• How to drill and face mill using table type horizontal boring mill
• *NEW Dura-Mill 5/8" 3 Flute - 60° High-Helix Carbide End Mill
• Center Dex mill/drill/bore tool, Mini-Mill chamfer too
• taig conversion, servo encoders reccomendation
• 2.5 D reccomendation

[cnczoner]

I believe IMTS is coming up in June. Take a few samples and you'll be overwhelmed with info.

Cheers,
-Neil.

[Ken_Shea]

Paul,
Obviously open to others opinions and arguments, however, Haas is an excellent choice.
For that size material the Mini Mill would be a good choice but with the Z axis extension. More than enough power for steel.

Haas has a wonderfully control, one of the more affordable CNC mills, made in the USA also very popular, consequently, lots of helpful information is available should or when you may need it.

Ken

[9 1/2]

http://http://www.imts.com/

[Geof]

What Ken says .

To compare with your .07" DOC at 6 ipm I do cold rolled or hot rolled at up to 0.20"DOC and 20 ipm using a 5/8" dia. four or five flute cutter, and compared to some people I think I am being conservative.

And, as Ken says also, the Haas control is very friendly.

[DSL PWR]

Without a cad file to go over I'd say it would take about 30 min for one piece on my TM-1. Since it looks like that is a 2 sided piece you could make a fixture for it and get 2 on the table. (1st op on one, and the 2n'd op on the other) So every hour you would have 2 complete flanges. This is with conventional tooling.

I'd run my 3/4" CIEM at 18-20ipm with a .17" doc. @ 3055 rpm. Then I'd go in with the fattest solid carbid mill I had for the finish pass. (providing I had enough room)

Now since you are doing lots of parts It's time to look at a hi feed endmill. I just got a 1.25" hi feed from Ingersol. Most of the time I can double my material removal rate. This sucker goes at 1300rpm (about 420sfm) with a .035" DOC at 100 ipm (this is in 1045). This gives about a .04"/tooth chip load. It seems to work best with up to 70% WOC, and I need to go to .02" DOC if I take a full pass. For your project I'd look at a 1" hi feed cutter (I know Walter makes them).

The problem with the conventional CIEM is the machine just isn't ridgid enough to use all of the hp. I personally an running a Mitsubishi AQX 3/4". This cutter would be able to do your profile in 1 pass with a bigger machine. But on an entry level machine like mine it starts to shake it's self to death, and with the death rattle come's blown inserts. With the hi feed there is still some vibration, but it is tolerable, and I get great cycle times.


So If I were you I'd took at a mini or a TM-1p. For a few grand more on the TM-1p you get pretty much the same machine, with double the y axis. Yes I know it's a little slower, but you don't have the rpm to make use of the speed any way. I'm guessing if you are doing turbo flanges, you may also get some bigger parts in the future. I know the smaller table would kill me, as I typically keep a vice on one side and a chuck on the other. Also remember that even with the 4" riser you will run out of z pretty quick on the mini.

I've had my TM-1 for nearly a year, and for about 6 months I've been cursing myself for not getting the tool changer at the very least, and a better enclosure would also be nice, with a chip auger...

Also remember not to cheap out on tooling when you get the machine, the extra capabilities won't gain you anything with poor tools. Since I've bought my mill I've spent about $15 000 on tooling. I've said it before, and I'll say it again, these tools are more expensive than drugs!

Good Luck

[jalessi]

Have you concidered a water jet, it might be the perfect solution for cutting your exhaust manifold flanges.

Jeff Alessi
jalessi@aol.com

[DSL PWR]

Have you concidered a water jet, it might be the perfect solution for cutting your exhaust manifold flanges.

Jeff Alessi
jalessi@aol.com

The problem with that is these flanges have some extra profiling in them, so he'd still need to mill them.

[Geof]

pauls; I have a question for you. You use 1/2" cold rolled and machine at least one face as well as pockets. Does it distort and if yes by how much? My experience with cold rolled is that if you take say 1/32" to 1/16" off one side of a piece of cold rolled about 14" long at will curl at least 1/32" over its length. Do your flanges do that.

[cnczoner]

IIRC some of the major exhaust header manufacturers in the US will CNC plasma-cut the basic shapes first, then mill them to the final size and features.

[DSL PWR]

IIRC some of the major exhaust header manufacturers in the US will CNC plasma-cut the basic shapes first, then mill them to the final size and features.

This does work, but I hate cutting thru flame cut material. Most of the time it goes ok, but there is always a couple parts where you hit a hard spot, and BANG!!! there goes your inserts, and very shortly after your tool. I nearly cry every time I try friction welding...

[jalessi]

There must be a much faster way to rough out these parts using some technology other than a mill. You guys are the experts!

[Geof]

This does work, but I hate cutting thru flame cut material. Most of the time it goes ok, but there is always a couple parts where you hit a hard spot, and BANG!!! there goes your inserts, and very shortly after your tool. I nearly cry every time I try friction welding...

You should do a cost benefit analysis. Abrasive water jet cutting is more expensive than plasma or flame but if it saves you a few multi-hundred dollar tools it may be worth it. Or a compromise may be laser; I think it is in between cost-wise but it leaves a more predictable, and thinner, heat affected zone; thin enough that you might be able to get completely underneath it in a single pass and if you use conventional not climb milling your cutter is coming at any hard spots from underneath.

[Geof]

There must be a much faster way to rough out these parts using some technology other than a mill. You guys are the experts!

As DSL PWR points out it is handling the stuff after it has been roughed out; sometimes that can be rough.

[DSL PWR]

There must be a much faster way to rough out these parts using some technology other than a mill. You guys are the experts!

The fastest and cheapest way to rough these out is plasma or oxy/fuel. The problem with these are stated in my last post. Water jetting them would work, but it is slow, and expensive. Laser cutting takes different plate, and is still quite expensive on thicker material.

Now lets say we find a cheap, and good way to rough them out. The only way to hold that profile for facing would be with 2 vices with funky soft jaws milled to the profile. Even with the soft jaws you won't be able to mill the outside profile.

When you start with flat bar you set it up in 2 vices (hey, it's 14" long!) and drill your holes. Once you have your run of stock all drilled in the right spots, you make a fixture plate on the mill. In this case it would be very simple, as you would only need to tap some holes in the right spot on the plate and bolt down your stock. You could probably squeeze 4 pieces on a TM-1 table. Now that you have the fixture bolted to the table, and the parts bolted to the fixture, you have one stiff setup, and you can flat out move while cutting. If Paul is welding some pipes to the back side of the flange, the benifit of cold roll is there is no mill scale on it so he shouldn't need to grind, or face mill the weld side. With the other methods he would need to face both sides of the part as a belt sander doesn't fair too well against mill scale (the various oxide grits are only about as hard as the scale on hot roll), and a side grinder would look like hell.

So for speed, cost, and simplicity I vote for the cold roll. Once every thing is dialled in the mill will run unattended for 60-90 min (if he springs for a tool changer...)

[rschap1]

I would just add (as my 2 cents),:
I don't see anything wrong with the entire part being done in a mill op. Use the right efficient tooling and cycle time will work w/o additional load/unload/set ups/handling. My employer is totally sold on Haas stuff. We have had poor luck squeezing into their Mini Mills with much of anything. I was stunned by the low cost of their "tool room" series though. My thought is to look at those. Good luck with them.

[Geof]

...... We have had poor luck squeezing into their Mini Mills with much of anything. I was stunned by the low cost of their "tool room" series though. My thought is to look at those. Good luck with them.

Yes the MiniMill is small, but before getting a TM it really would be worth doing a test on the two machines. The MiniMill has faster rapids and is stiffer than the TM this could make heavier cuts possible.

[neilw20]

All the fancy shapes in a male and female tool.
Bright Red Hot.
Big Squeeze. Finished shape.
Time cycle with good furnace would be heaps fast.
Allow for shrinkage. Surface grind finished faces on big wash grinder. (3 minutes)
Will this work?

[pauls]

Tried the plasma cut route with my cnc plasma cutter. Speeds up the process some but adds another step and the hard spots here and there are brutal on the end mills.
Thanks for all the input. I'll have to do my homework and checkout the available machines.
Paul

[big_mak]

If I get PArts that have been flame cut, I use conventional milling to get under the scale, then you don't have that hard impact on the tool. I'll Also use lots of Plunge Milling!!!!!! There are ways to limit the damage of the HAZ.