CNC Tooling

[Cory]

Originally Posted by MICHAELABICK

For workholding we are thinking of getting 2 Kurt 3600V vises. Because the table on the TM-2P is so big I'm not sure if it would be beneficial to get 3 vises. I've heard good things about glacern too so we are still deciding between the twoo. Workholding seems like it is a very good area to invest in.

For CAM I've heard good things about mastercam from the CD community but our haas rep recommended gibbscam. I'm still not quite sure which one to get.

I found these drill bits on mcmaster: http://www.mcmaster.com/high-speed s...gth drill bits. They say good for steel, cast iron, and plastic and they are 118*, but I assume they will be fine.

Are 90* spotting driil okay? I've heard that your spotting angle should be bigger than your drill bit angle.

For toolholding I want to get at least 4 1/4" EM holders and 4 1/2" EM holders. I'm still not sure if I want to get 1/8", 3/16", and 3/8" EM holders. I want 14-16 ER16 tool holders, 1 drill chuck, and 1-2 face mill arbors.

4 each of 1/4" and 1/2" end mill holders is a lot. We only have 2 of each. You don't want to use a solid holder for 1/8" end mills. Any runout will destroy the tool in short order. Use a collet.

14-16 is a lot. It's taken us 5 years to accumulate that many and our machine can hold more tools. I don't know that I'd start out with so many. I'd also add a few ER-32's. You're going to want them to hold any drills/end mills over 1/2", or even 3/8" for rigidity purposes.

I don't really see a need for 2 face mills-just get one that takes standard inserts that are available for ferrous and non-ferrous materials. I'd rather have 2 drill chucks.

The drills you found are fine. 90* spot drills are fine.

The more vises you get the better. 3 vises means you're 50% more productive if you're making multiple parts. I would buy 4 of the Glacern 3600V clones over 2 3600V's.

Again, all of this comes back to your budget. This is all a "price is no object" list without one. If it's tight, lots of things I've suggested can be cut back to the bare minimum to get up and running.

[craigboez]

Originally Posted by Cory

Corner radius is always preferred if you don't need a square shoulder. The number one reason end mills go bad is the corners of the flutes chip and then the cutting edge gets destroyed. Corner radii help prevent this.

I thought I'd revive this excellent thread from the dead. Getting ready to purchase some new tooling, and I see there are usually several options for the amount of corner radiusing. For example, Maritool offers .008, .015, .030, .060, and .090 radius options for a 1/2" endmill. Never having purchased one I'm not sure why to choose one over the other. I'm assuming that the biggest radius will lengthen tool life the most, and since we are mostly doing thru-cuts on everything the radius will never have an impact on the cut geometry. Anyone care to elaborate on this?

[Cory]

Originally Posted by craigboez

I thought I'd revive this excellent thread from the dead. Getting ready to purchase some new tooling, and I see there are usually several options for the amount of corner radiusing. For example, Maritool offers .008, .015, .030, .060, and .090 radius options for a 1/2" endmill. Never having purchased one I'm not sure why to choose one over the other. I'm assuming that the biggest radius will lengthen tool life the most, and since we are mostly doing thru-cuts on everything the radius will never have an impact on the cut geometry. Anyone care to elaborate on this?

You have it right. Larger radius will reduce the chances of edge chipping and increase tool life.

[mman1506]

Would you mind sharing some fixturing techniques Cory? Are team is trying to figure out the best way to mill gearbox side plates.

[sanddrag]

Although I'm not Cory, we usually put a good size tooling plate (just 6061 plate, about .75" thick or so) in a vise and face mill it to level it out. Then we run a program to drill and tap that fixture plate with our hole locations for our gearbox plate. Then we clamp 1/4" plate to that with little C clamps, then we drill the 1/4" plate only barely through, using the same XY part zero offset. Then we remove the clamps, bolt down the plate, and do all the pocketing and cut the outside profile.

[Cory]

Originally Posted by sanddrag

Although I'm not Cory, we usually put a good size tooling plate (just 6061 plate, about .75" thick or so) in a vise and face mill it to level it out. Then we run a program to drill and tap that fixture plate with our hole locations for our gearbox plate. Then we clamp 1/4" plate to that with little C clamps, then we drill the 1/4" plate only barely through, using the same XY part zero offset. Then we remove the clamps, bolt down the plate, and do all the pocketing and cut the outside profile.

We do what Dave said, with modifications. If the plate is small enough to be clamped in a vise (less than 17" for our vises), we'll clamp the plate in the vise, drill and tap all the holes in it, then load up a fixture plate and drill and tap through a subset of the holes drilled in the actual part in the first operation.

Another alternative that works well for smaller (roughly the size of our drive gearboxes) is to do everything in one operation, in a vise, and leave tabs connecting the part to the stock when contouring the outside. After you're done you can cut the tabs and sand them flush with the outer contour. If you're careful and you follow the sanding with scotchbrite you can blend the contours very well.

[Mk.32]

Originally Posted by mman1506

Would you mind sharing some fixturing techniques Cory? Are team is trying to figure out the best way to mill gearbox side plates.

A more quick and dirty solution is, I have just taken 1/4 6061 and clamped it to the table of the machine with a hunk of 3/4 ply wood in between. Then drill my though holes, and wood screw the alum plate to the chuck of wood. Then do all the inside/outside cuts, pop the screws and you have your part.

[scottandme]

Originally Posted by Mk.32

A more quick and dirty solution is, I have just taken 1/4 6061 and clamped it to the table of the machine with a hunk of 3/4 ply wood in between. Then drill my though holes, and wood screw the alum plate to the chuck of wood. Then do all the inside/outside cuts, pop the screws and you have your part.

We run more or less the same setup, but we use acrylic as backing and double-sided tape instead of retaining tabs or screws on the part.

Just tape the part to roughly the same size scrap acrylic (we use 9mm), and strap clamp the part onto the table. We generally run a 1/4" 3 flute high helix end mill with 0.1" deep passes. With that you don't have to worry about chip evacuation in the slot, and it leaves a thin final pass (0.025" in 1/8" and 0.05" in 1/4"). Then just take the whole plate out of the mill, hit it with the heat gun until the tape releases, and then assign freshmen to a character building deburring/scotchbriting.

Mitee-bite sells a similar product that leaves less residue, but you have to heat the part to apply and release the compound. Double sided tape seems to be cheaper and faster when you have students to help. It's McMaster number 50245A21.

Otherwise just check out Mitee-Bite or Carr-Lane and poke around, they have lots of interesting stuff for fixturing. We tend to just do a lot of simple parts in the vice, the double sided tape method, and rarely a part using soft jaws. Two vices are helpful for long parts to minimize vibration/chatter, just indicate them in and clamp your part.

[DonRotolo]

I'm fairly accomplished with manual mills and lathes, but I am almost done building a 27" x 50" CNC router, and I'd like some advice on tooling and cooling. The driver here is a Hitachi 2.5 HP variable-speed router, with a range of about 8000 to 24000 RPM and 1/4 and 1/2" collets.

I see many choices of straight bits for cutting aluminum. Any suggestions on what to look for / at, brands that seem to work well, etc.?

In my manual milling and turning world, coolant use is rare. Just don't need it for most materials. But in the CNC router world, I fear that coolant is almost always used. Anyone have time to help me drink from that firehose? Not just coolants themselves, but ways of applying it, collecting, filtering out the chaff, etc. I don't even know what I don't know yet...

[AdamHeard]

Originally Posted by DonRotolo

I'm fairly accomplished with manual mills and lathes, but I am almost done building a 27" x 50" CNC router, and I'd like some advice on tooling and cooling. The driver here is a Hitachi 2.5 HP variable-speed router, with a range of about 8000 to 24000 RPM and 1/4 and 1/2" collets.

I see many choices of straight bits for cutting aluminum. Any suggestions on what to look for / at, brands that seem to work well, etc.?

In my manual milling and turning world, coolant use is rare. Just don't need it for most materials. But in the CNC router world, I fear that coolant is almost always used. Anyone have time to help me drink from that firehose? Not just coolants themselves, but ways of applying it, collecting, filtering out the chaff, etc. I don't even know what I don't know yet...

I'll leave others to comment on tooling, but I will say we run a mister nonstop during cutting. It greatly increases cutting speed and reduces failures. This doesn't create a lot of liquid per hour, so we don't have any method of collecting or reuse for it.

[mman1506]

Originally Posted by DonRotolo

I'm fairly accomplished with manual mills and lathes, but I am almost done building a 27" x 50" CNC router, and I'd like some advice on tooling and cooling. The driver here is a Hitachi 2.5 HP variable-speed router, with a range of about 8000 to 24000 RPM and 1/4 and 1/2" collets.

I see many choices of straight bits for cutting aluminum. Any suggestions on what to look for / at, brands that seem to work well, etc.?

In my manual milling and turning world, coolant use is rare. Just don't need it for most materials. But in the CNC router world, I fear that coolant is almost always used. Anyone have time to help me drink from that firehose? Not just coolants themselves, but ways of applying it, collecting, filtering out the chaff, etc. I don't even know what I don't know yet...

We have a mister that looks just like this one on are diy CNC http://www.cnccookbook.com/CCMillCoolantMister.htm
I'm not sure where we bought it but it connects to a 20 psi air line and another hose goes into a coolant bottle. It uses a venturi to suck up the liquid. Since it uses compressed air it also helps blow chips out.

[sanddrag]

On our router at ~20,000 RPM, we've had a lot of trouble cutting aluminum with a standard 1/4" 3 flute carbide variable helix endmill we use with great results at 6,000 RPM with coolant on the mill. On the router, it just wants to load up and melt/weld chips. I'm thinking a 2-flute would give better chip evacuation.

Currently, our coolant system on the router is a student and a spray bottle of WD40.

[R.C.]

Originally Posted by AdamHeard

I'll leave others to comment on tooling, but I will say we run a mister nonstop during cutting. It greatly increases cutting speed and reduces failures. This doesn't create a lot of liquid per hour, so we don't have any method of collecting or reuse for it.

Originally Posted by sanddrag

On our router at ~20,000 RPM, we've had a lot of trouble cutting aluminum with a standard 1/4" 3 flute carbide variable helix endmill we use with great results at 6,000 RPM with coolant on the mill. On the router, it just wants to load up and melt/weld chips. I'm thinking a 2-flute would give better chip evacuation.

Currently, our coolant system on the router is a student and a spray bottle of WD40.

David,

Like Adam we also use a mister non stop. Your issue is using the WD-40 squirt bottle. Its a waste of time, we did that for a few weeks until we got tired of endmills gumming up and wasting our money.

What we also do is a run 2 airlines + the mister. So two airlines are blowing away the chips so your not recutting chips. The mister keeps the endmill from gumming up.

http://littlemachineshop.com/product...y=212208195 9

This is the one we have, bought it off of ebay for ~$40 bucks.

-RC

[DampRobot]

We use a mister too. I'm not sure of the model. It does help a significant amount, we've been able to cut faster after starting using it (I think we started out at like 2 in/min with a 1/4" cutter in 1/4" alu before, now we set it to 6 ipm fairly regularly). In my experience, mist coolant helps most with cutters in the 1/4" to 1/2" range, where heating tends to slow down your cutting speed. With very small cutters (1/8" or smaller) I've seen them break more because of their small diameter than whether or not coolant was used.

Like others have said, collection or recycling isn't really an issue as the mister doesn't put out much fluid. However, it's very important to clean up properly after using the coolant. A lot of our steel tool holders have noticeable rusting in small spots from the mist, and after some pooled under our vise, it left a mark on the machine's table. I recommend wiping down the machine well every day, and taking up any fixtures on the table every week or so. On the other hand, it's a good idea to do this anyways.

8000 is extremely fast for tools in the 1/4" or 1/2" range, in my experience. With coolant, I believe we typically set 1/4" two flute cutters at 2000 rpm or so in 1/4" aluminium at a feed rate of about 5 ipm. Our mill only goes to 3600 rpm, and we only really use it that high for very small tooling.

[Cory]

Originally Posted by DampRobot

8000 is extremely fast for tools in the 1/4" or 1/2" range, in my experience. With coolant, I believe we typically set 1/4" two flute cutters at 2000 rpm or so in 1/4" aluminium at a feed rate of about 5 ipm. Our mill only goes to 3600 rpm, and we only really use it that high for very small tooling.

A 1/4" diameter carbide end mill under ideal conditions wants to be run between 12,000 and 36,000 RPM (750-2000 SFM).

At 2000 RPM you're at 125 SFM which is fine for HSS but doesn't take advantage of carbide's benefits.