Thread: What Feed Rate? Speed etc?

First up, a compression bit is wasted on what you're doing. The up-cut section is 7/32, which leaves just 1/32 down-cut in your 1/4 plywood which won't be much help with reducing breakout. A normal up-cut bit would have been a better choice and probably a fair bit cheaper too. Sorry to be "that guy", but if you want to get the most out of your CNC for the lowest cost, you need to be aware of this stuff.

Now on to the answers. A lot of it is calculated from the Onsrud router bit catalogue ( https://www.onsrud.com/files/pdf/OC-...oolCatalog.pdf ), it has comprehensive feed charts for all different materials. It can be daunting to navigate, but use the contents pages at the front to find which bit best matches the one you have, then use the catalogue number of the bit to go through the chart at the back that suits the material you're using.



How deep would you cut in each pass? You can do it in 1 pass

Stepover? Manufacturers of milling tools for metal recommend 70% of the cutter diameter, this number seems to work well with timber as well

Spindle speed? It will do 24000 rmp at 800w. Full speed

Feed rate? 5500 mm/min is what the charts say, but I'd probably stay around 3500-4000 mm/min

Plunge rate? 3000 mm/min

Will I need a ramp? You don't have to for this, but I'd highly recommend it when using compression bits at a depth that will use the down-cut section.

I read it is best to climb in direction. That's a tricky one. I like climb cutting solid timber to reduce breakout, but I've found that climb cutting where the whole width of the bit is in the material (like nested components on MDF/ply sheets) gives a worse finish and is not dimensionally accurate. It's not out by much, but for clock gears I'd suggest cutting in the conventional direction just to be sure

What length and thickness of tabs. Can't help there, never had to do it

I know this is a lot but I am a real newbe. I am hoping for rule of thumb numbers on this. http://www.amanatool.com/media/custo...1435768257.pdf

Hope that helps

G'day Mike... You could ask 10 people and get 10 different answers (all of them correct), so here's what I would do -
Considering your 1/8D at 2&1/2" long bit will flex

How deep would you cut in each pass? - I'd do it in 3 ramped passes, but a single pass is possible

Stepover? - Normally I keep stepover to 60% max, but prefer 50%

Spindle speed? It will do 24000 rmp at 800w. - 24k would be normal, but I adjust the spindle speed during the cut until it sounds sweet but still keep the max revs I can.

Feed rate? - I would use 1200mm/min, but that's an ideal speed for my machine. I find it's the best speed for my setup

Plunge rate? - Again, 1200... but that's perfect for my setup

Will I need a ramp? - I'd use a spiral ramp because it will reduce your witness marks and will cut a better finished edge

I read it is best to climb in direction. - For what you're cutting, I would climb cut with a spiral ramp to 2mm depth at 0.15mm offset, then do a conventional cut at full depth and no ramp to the finished size.

What length and thickness of tabs. - On your material and job, I wouldn't use tabs. Here's how I would tackle it... A couple of glue dabs on the back of the gear to hold it down to the spoil board to stop it twisting as it's being cut, plus finger clamps around the outside, then cut the center hole and put a screw to hold it down when the gear is cut out. This means that when you finally cut the gear out, the screw holds the gear down (the finger clamps will no longer give any support) and the glue will just hold it in rotational position.
Rough cut the gear (climb) and try to leave a 1/4mm (or less) skin cut without tabs. Finish cut (conventional) to full depth and the gear will be fully cut out. Remove the finger clamps, the waste will come away... remove the inside screw and slip a knife under the gear to break the glue dabs. Sand/scrape the glue dabs away and you'll have a perfect gear. The reason I wouldn't use tabs is that it will be a mess to try and break out the tabs afterwards, so it's much easier to hold it in the center and do away with the tabs 'problem'...

Hope this helps too

It does help a lot - thank you.

Hi Mike
All of the above info is good, but the most valuable info will come from doing your own tests with the specific material on your machine.
My machine works better when it runs a bit slower and does more passes (and the relatively inexpensive end mills also appear to last longer).
You'll find machining ply is particularly heavy on whatever bits you use.
Another tip for improved edges is to remove the bulk of the material with an offset and then doing a final pass at zero offset and at full depth.

There are a batch of good ideas in the previous posts, the only things I can suggest as an addition would be to use a heavier more rigid bit to do the actual cutting (oversize) to full depth then use your mini compression to take things to finished size and profile. This should give you better bit life for the mini comp, with a lot less chance of breakage, at the expense of having to develop two sets of paths for each gear and a bit change midway.If the mini comp bit will be barely into the down cut for the top surface as Elan suggested, I would use an extra skimmed MDF spoil board under the gear and let the mini comp cut 1mm or so into that board. Once the hard surface has been skimmed off the top of the extra spoil board, the soft core should not load the mini comp too much particularly if it is only trimming small amounts from the gear blank in the final pass.Oh, one final thing, the finish of the gears you cut will ultimately be limited by the quality of the ply you use for a blank, junky 1/4in 3ply with a coarse grained skin will not give anywhere near as good a gear as one cut from 7ply aircraft grade birch, but it will be a lot cheaper.