Feed and speed number help

Technical Manufacturing
1

I just purchased the 4mm end mills from WCP for our CNC router. I see a ton of postings on feeds and speeds but nothing all in one place and complete. I was wondering if I could get answers to a couple of questions as our team is having a hard time using our new router, and the kids and I keep breaking bits and getting a ton of chip welding in the slots.

Our team has a 4.08hp spindle on our 4x8’ techno hd that can range from 6000-18000rpm.

We are planning to use the 4mm bit to slot out profiles in 1/16", 1/8", 3/16", and 1/4" thick 6061t6 aluminum sheets. (for typical gussets, gearbox plates, hole patterns, etc). What feed, speed, plunge rate, and doc would you recommend for each thickness using the 4mm bit? Can we do each thickness in one shot, or do multiple passes at whatever recommendations you provide?

Also, if we want to do hole patterns for a #8 or 5/32 rivet using the bit, what feed, speed, plunge rate, and doc would you recommend?

We are usually screwing down the aluminum plate, and/or using double sided tape for work holding. Also we have a vacuum and cold air gun that are running as well.

Lastly, we have been buying the two bits below, but keep getting bad results (edge breaking down, tons of chip welding in the slots .Would you have any recommendations on the same processes mentioned above, but for 5/32 and 1/4 diameter?

https://www.amanatool.com/51473-soli...outer-bit.html

and

https://www.amanatool.com/51479-soli...outer-bit.html

Armana recommends 18000rpm at like 80ipm which seems fast…we tried the 1/4" at those speeds with a 1/8" doc. Still were getting crazy chip welding in the slots when doing profiles. Maybe those numbers are totally of base?

Thank you so much everyone for you sharing your expertise.

Stephen Peroni
Mentor - Team 3950

2

What CNC router are you using? EDIT: I’m blind

Are you using any coolant/oil/mist?

Techno isn’t the stiffest machine, the main thing is to avoid any chips lingering in the cut. CHIPS ARE BAD. those amana numbers are not for a CNC Router, they are for a CNC mill. 0.125 is very deep for a router, crazy deep for a slot pass. I would start at 20 ipm.

3

Just a fair warning; I do a lot more CNC milling than router work so take my advice as you will. If you take your depth of cut down to about 50 thousandths and give the cut some air (as easy as a freshman with an air hose), you should eliminate your chip welding problem. Also, you may want to stray away from using tape as a Work holding device.

4

Start with an IPM recommended by the manufacturer. For example, 80ipm might seem fast, but if you use a low depth of cut (like .02", for example) it would be very difficult to break the tool. It’s important to follow chipload recommendations from manufacturers, or you’ll prematurely wear the tool. Going too low of an IPM will cause more rubbing than cutting, which makes the tool heat up faster.

For the WCP 4mm endmills, they recommend .002 to .004 IPT. That means for a 16k rpm spindle speed, you’ll want 16,000*.002 = 32 IPM minimum, and 64 IPM maximum. Start at maybe 38 IPM and a .05" DOC - that’s close to what I regularly run on cheap Aliexpress endmills. The Amana 1/8" can be run at a similar starting point.
You can probably use the 5/32" or 4mm bits to go through 1/16" sheet in one pass, and I’ve heard of people doing the same with 1/8", but start off simple with a .05" or .04" DOC and work your way up from there. Workholding properly (see below) is the most important thing.
Once your slotting parameters are dialed in and consistent, you can think about using adaptive strategies with high DOC and low WOC to maximize tool life.

EDIT: your links are broken, but use this guide to help you find the recommended IPM/RPM if you haven’t seen it already: https://www.amanatool.com/pub/media/custom/upload/File-1476280931.pdf
For the 51473, it seems to recommend a similar .002-.004 IPT. The 4179 recommends .003-.006 IPT, but the 4mm is arguably a lot more useful, so get that dialed in first. That being said, 1/4" single flute endmills are incredibly robust- we had to fall back on one during the 2018 season for our Tormach CNC, and it hasn’t broken yet (through 2 robots’ worth of parts!). So if you still have trouble slotting even with the air blast, try the 1/4".

Make sure your plates are held down well. Take a large sheet of aluminum, drill/bore any holes you need in you parts, then screw the parts down with the holes before doing cutout. Double sided tape works, but I find that it can be a pain to remove. Home Depot/ Lowes sells little flathead phillips brass screws that work really well; The #6 size works for most holes. Make sure you use as many screws as possible to maximize rigidity!

I haven’t worked with a Techno before, but from a couple videos I can see it’s got a pretty rigid construction and linear guides, plus what appears to be an actual rectangular spindle (as opposed to the usually cheaper circular ones).

5

Thank you so much everyone. I spoke with RC from WCP and they run the 4mm at 14,000 and 30-35ipm with a .06 to .09 doc, and plunge of 5ipm.

I think we have been trying to do too much doc and our chip evacuation is a problem…right now we are running an exair cold air gun, and have a vacuum hood around the bit… depending on our results with the new feeds/speeds, we will look into a fogbuster and/or air blast to aid in chip evac.

Thank you all again…i hope this thread helps out others in the same situation.

6