[iWAYNE]

OK, its time to get a CNC router to boost production, but I need advice on how much spindle HP I will need to get good production rates without overdoing it on the cost for more HP.

I work with 1/2" thick HPDE plastic and want to be able to cut thru in one pass and not repeated passes. Basically I need to route plastic flange disks 6.5" to 9" dia with bolt holes.
I'm talking to a router manufacturer who has a machine with a 7.5 HP spindle, and 11 HP is also available as an option. He isn't familiar with cutting HDPE so he can't give me advice on this issue. Is 7.5 HP enough to route in one pass in 1/2" HDPE, or do is the 11 HP needed?

[inventor83]

Well. 7.5HP would do the job but at a slower feed/spinde speed. If you want maximum feed rates(providing your machine rigidity is there) then go for the 11HP.

The question is not if a 7.5hp spindle can do it, it can... Just how fast.

[iWAYNE]

Thanks, I guess the question is how much slower? The manufacturer offered to test it on one of his machines if I sent them the plastic sheets. That may be the best way to know.

[alan_3301]

according to a popular calculator,
with a 1/2" carbide 2 flute endmill, full slot and full depth, spun @ 9317rpms feeding @ 292 ipm with a 0.0157 inch per tooth chipload would require 6.4 HP.
with a 1/4" carbide 2 flute endmill, full slot and full depth, spun @ 14394rpms feeding @193ipm with a 0.0067 ipt chipload would require 2.1 HP, however deflection would be too large @ 0.002"

I think it will depend on the bit size you choose, and how much power is available at different spindle speeds?
maybe that helps.,

[ger21]

I think you'll find that 7.5HP is more than enough. A more important issue is how to hold the discs in place.

[iWAYNE]

It has a vacuum table. Laguna Tools with 5'x10' table.
Smartshop 5x10 CNC Routers

I've been ordering them routed out by the plastic distributor for years, but will be cutting my own soon. They use vacuum tables to hold the sheets down.

[iWAYNE]

Alan, can you give me the name of this calculator, or a link? I'd be interested in looking at it. One of my suppliers did say they used a 1/2" dia bit for routing them which surprised me. It seems like a lot of wasted material cutting out disks on a sheet.

[inventor83]

The 'wasted material' becomes less of an issue when you consider deflection. A 1/4 inch bit will most likely break under those loads. You could always take 2 passes at the disks using a 1/4 inch bit. It may work out better to do this and save yourself from buying the 11hp.

Your cut quality might suffer by trying to cut it all in one go. You may need more vacuum power too. This is something you really need to just test for yourself and decide what works best.

[iWAYNE]

Talking to the router manufacturer today, he said almost the same thing. You can "hog" your way thru it in one pass yes, but the finished edge will not be good. Best to make one rough pass, then a finish pass. Their engineer said 7.5 HP was fine for my needs, but talking to the production manager at a plastic supply that I use he said he'd suggest going for the 11 HP spindle instead of the 7.5HP spindle. That surprised me. At least with 2 passes I might be able to use the 1/4" bit which I would prefer, but it will be trial and error for all the factors involved.

I also was told that the 5'x 10' table needs a second vacuum pump because of its size, so (2) 10HP pumps for this. Also they recommended a 4.5 HP chip collector, 3 HP at the bare minimum.
Thanks for the input from everyone. Its been very helpful.

[ger21]

If you use a 1/4" bit, you can probably get away with 3HP. No way you'd need anywhere near 7.5HP, unless your cutting very aggressively, with a 1/2" bit.
You probably want to use a 3/8" bit, which is a good compromise for speed and rigidity.
Do you have an ATC? If so, I'd use a roughing bit, followed by a finishing pass with a finish bit. A roughing bit can cut much faster, with much lower cutting force. And it'll last a long time, and allow the finishing bit to stay sharp for much longer.

Are you vacuum holding these through an MDF spoilboard?

[iWAYNE]

Yes this router comes with an ATC. The roughing bit is a good suggestion, thanks.
I will be using an MDF spoil board, yes. I'd like to bolt it down in the t-slot instead of gluing it. Does anyone know who makes the nylon bolts for this?
I will need to figure out how many bits I'll use. So far it looks like 4. I need one to make a 1/8" deep recess cut 4" dia in the center of a 9" disk but not sure which is best for this. Any suggestions on the best bit size for this part? I wondered if a 4" fly cutter would do the job since its such a shallow cut.

[bhurts]

Fly cutters are a big no no in a router. You can use a insert cutter instead.

Ben

[iWAYNE]

By fly cutter I mean a spoil board surfacer like Amana:
Industrial CNC Insert Spoilboard Router Bit with Scorer 2+2 Design by Amana Tool

They don't have a 4" dia model, but you don't think this could do the recess cut, plunging 1/8"?

[ger21]

No, you can't plunge with those. Just do a pocket with the roughing tool. You should be able to cut it at a very high feedrate.

[iWAYNE]

Looking at the Amana bit site, they say the roughing tool need 20,000-21,000 rpm. The 7.5 hp router I'm looking at is only rated at 18,000 max.

[ger21]

You don't have to run tools at any specific rpm. Depending on feedrate, you probably want to run it in the 14,000-15,000 rpm range.
What you want to do is use a rpm and feedrate that gives you an optimum chipload. Amana doesn't give a lot of chip load info.

Go to http://www.onsrud.com/xdoc/FeedSpeeds
and find a similar tool, and use their chip load charts to calculate rpm and feedrate.

[iWAYNE]

I also need to decide on CAM and nesting software for this router. Does anyone have any suggestions?
Even good open source is OK with me.

[iWAYNE]

I can tab the disks if the vacuum table doesn't quite have enough umph.

[daniellyall]

A 3/8 or a 1/2 bit should fly through with a 7.5 hp spindle it should be able to do 1/4 in one go just play with some scrap wood to get the feed and speed correct have a look at a few speed and feed charts or a speed and feed calculator, some are way off the first one I used was that far of I was breaking and burning out cutters way to fast in rpm (it was from the manufacturer of the cutters I was using).
for cad doing woodwork vcarve pro is pretty good