CNC Newbie looking for advice

lcorley

lcorley

Registered
Registered
Joined
Nov 16, 2014
Messages
56
Hey guys,

I recently bought a Taig CNC setup. I'm using Mach3 in demo mode till I figure out what I want long term. My first two projects were a spindle wrench for the Taig and a spanner wrench for my spin indexer. I cut these out of 1/4" aluminum sheet. I used Fusion 360 to design the parts and generate the toolpaths. I chose a 2D contour cut with a 1/8 inch flat end mill. I used a 0.020 stepdown so it cut the part out in 13 passes. I could only get about 3-4 inches per minute feed at 6500 RPM without risking the chips loading up and breaking the bit. I feel I must be doing something wrong -- I expect better performance. Can anyone offer some advice, or point me toward some basic tutorials on tool paths and "recipes"? Thanks in advance.

regards,
Leon


wrenches.jpg
 
What coolant were you using? Kerosene is my favorite for aluminum, but WD-40 works well also.
 
I was using WD-40 part of the time, and cutting it dry some of the time. I couldn't tell much difference.
 
Last edited:
2 or 4 flute endmill?

To answer your question, the way I have always done it is to experiment with feeds and speeds until it's cutting like I want. I normally run the spindle slower than the charts, but keep the chip load in the proper range. In the case of a 1/8 end mill, about 0.0009 / tooth, a 1/2 endmill I might bump the tooth load to around 0.003 or so. Normally use a 2 flute on aluminium, especially in smaller endmills because you need more chip clearance and you need to keep the tool wet with coolant.
 
You might want to look at https://www.cnccookbook.com. There are quite a few articles that will be helpful and G-Wizard (free for a short time) is one way to figure speeds and speeds pretty easily. Watch out for all of the email, push notices, etc they want to send though. (I've never had any spam, but they sure ask often if they can send stuff!)

https://www.autodesk.com/campaigns/cnc-handbook is a free cnc handbook by Autodesk that is worthwhile.

As far as the particular examples your depth of cut might still be a bit deep and the rpm too fast. It all depends on the type of endmill (carbide, HSS - 2 or 4 flute and amount of stick-out). A 0.125 endmill isn't real strong (as you've discovered). A lot of times if I am cutting profiles like in your pictures I will waste a bit of material and cut with a 3/8" 2 flute rougher leaving a few thousands profile, then do a couple of full depth finishing profile passes with the 1/8" if needed.
 
Using a 1/8" end mill is going to take patience. As you said you can't get too aggressive without risking breaking the end mill. I've never run a Taig but I do know they are a light duty mill. My suggestion is use a larger diameter end mill, say 1/4", and gradually bump up your speeds and feeds. The larger end mill is more robust and less likely to break which will give you more flexibility when setting feed rates. A ball park number for a high speed steel end mill cutting aluminum is 300 surface feet per minute. That's 9100 rpm for a 1/8" cutter. Start low and work your way up. And use coolant continuously and evacuate the chips. Try a Fog Buster.

Let us know how it works out. There is a huge knowledge base on this forum and we're here to help.
 
Thank for the responses. I'll try shallower DOC. and see if that helps. I'll also try a 1/4" mill. Do you think adding a Kool-mist would help with the aluminum chips in the deep slots?
 
Kool-mist will help by keeping aluminum from attaching itself to the endmill flutes. It is a good idea (especially for the finish) to keep chips from accumulating in the slots. For example, use flood coolant under pressure or compressed air to blow the ships out, even a chip brush if you can keep from getting the bristles hung up on the endmill (& watch your fingers!).
 
get ME consultant 2.0 for your speed and feed. adjust DOC to what your mill will take. You will find a certain size endmill will remove material the fastest on your machine. My guess would be a three flute 3/8 aluminum cutting endmill. a 3/8 two flute may be almost as good. you got to play to see what the machine will do
 
My experience with Kool Mist even using distilled water was that it stained aluminum parts. I tried talking with them to work it out, but it became an exercise in blame shifting. I switched to SC520 and distilled water and never looked back. The stuff is awesome. I'm not a big fan of Bob Warfield or G-Wizard, but any speed feed calculator is better than none. Currently I am using HSM Adviser and its very good, but perhaps not for a Taig. Zero (Eldar Gerfanov) assumes you have a rigid machine which a Taig definitely is not. I use pretty much all SF calculators as a ballpark jumping off point. I use ME Consultant Pro as a backup to double check when the numbers from HSM Adviser don't sound right.

There is a limited version of HSM Adviser available on-line for free call FS Wizard. FS Wizard is also available as a free (lite) limited version or a full version as a cellphone ap. The full version of the cell phone ap is free with a licensed version of HSM Adviser. https://fswizard.com/

ME Consultant Pro says with a 2 flute carbide you should have been able to slot at 9.19 ipm at 10000rpm.
HSM Adviser says 11.24 at 10K with a 2 flute carbide. I assumed more than optimum stickout.

At 6.5K they said 5.974 and 7.31 ipm respectively when slotting at .02 DOC. Sounds like you are about right. You might be able to slot faster if you chuck up close on the end mill, go to a three flute (4 flute has chip clearance issues for high speed machining in aluminum), and use flood coolant to blast chips clear.

With .3 inches stickout HSM adviser says you can run upto 17ipm on an ideal machine at 6500 RPM and 27ipm at 10K and 30ipm if you upgrade to a 3 flute. I really doubt it though. The reality is you probably can't do that with a Taig. Its a pretty flimsy machine. Its only .03 HP calculated load, but with the machine flex the load on the cutter will be a lot more.

When you upgrade to a 3 flute .250 end mill the suggested feed doubles, but the horsepower requirements increase by more. While a Taig spindle motor is rated at .25 or .33 HP depending on the exact model its not going to have the torque at the higher RPMs and you don't want to run your motor IMO at more than about 50% of rated power continuously. Also, remember, A TAIG WILL FLEX. I know I own one, and I used it way beyond its reasonable or even unreasonable limits. I ran mine at one time with two spindles cutting two parts simultaneously.

The big thing with aluminum is keeping the cut cool and blasting chips clear of the cut. SC520 works great. Koolmist 77 will work ok if you don't mind stained parts. The problem is Taig specifically says not to use a water based or water soluble coolant on their machines. Electrical risk may be one of the reasons, but the other is that a Taig is a composite machine made out of brass, aluminum, and steel. I suspect they are afraid of galvanic response between the metals in a wet environment. If you look on YouTube you will see guys are using water soluble coolants on their Taigs though. I asked a few how they were after a few years, and they said they were fine. I had retired my Taig when I switched to water soluble coolants. I used (you are going to laugh) flood transmission fluid on my Taig. It burned up over time on long jobs, but the cuts looked fantastic. Cleans up with soap and water if it needs to be "CLEAN" or wipes down with a towel if a little oil won't hurt it. The parts never stained.
 
You must log in or register to reply here.
Back
Top