# CNC Newbie looking for advice



## lcorley (Nov 28, 2017)

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


----------



## JimDawson (Nov 28, 2017)

What coolant were you using?  Kerosene is my favorite for aluminum, but WD-40 works well also.


----------



## lcorley (Nov 28, 2017)

I was using WD-40 part of the time, and cutting it dry some of the time.  I couldn't tell much difference.


----------



## JimDawson (Nov 28, 2017)

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.


----------



## Groundhog (Nov 28, 2017)

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.


----------



## TomS (Nov 28, 2017)

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.


----------



## lcorley (Nov 30, 2017)

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?


----------



## Groundhog (Nov 30, 2017)

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!).


----------



## Karl_T (Nov 30, 2017)

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


----------



## Robert LaLonde (Nov 30, 2017)

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.


----------



## spumco (Dec 1, 2017)

+1 advice to get HSM advisor or another F&S calculator.  A reasonably useful trick to using feed & speed calculators on less-rigid machines is to de-rate your spindle power in the program.  If the Taig has .25hp, tell the software it has 75% of that.  Also set your permissible tool deflection very low in the software for each cut.  Since the Taig is going to flex anyway, you don't want cutting deflection added to machine-induced deflection.

Also-
1. Largest diameter tool you can use (I suspect that's a 3/8" on the Taig, but others will know better).
2. Shortest tool you can use - buy stubby end mills and choke up on them as much as the cut allows.
3. Anything you can do to get the chips out - mist, air, flood - whatever.  Amazon has really cheap mist coolers for about $10-$20, even if they're terrible for siphoning the Kool-mist or whatever, they're good at blowing chips away.  If the tool stays cool, the chips won't stick to it as much.
4. Try cutting those parts with an adaptive tool path rather than slotting.  This keeps - usually - the chips from building up in a cut or slot.  You waste more material, but the tool lasts longer as it's taking an appropriately thick chip and the chips usually have an easier time escaping the cut.  

In the case of your parts, I'd model them with a couple extra holes for hold-down screws.  Take your stock and drill the holes while in the vise.  Remove stock from vise and drill a matching pattern in a chunk of aluminum held in the vise that was bigger than the parts.  Tap the holes and the chunk now becomes a spoil-board for your actual parts.  Screw the stock to the spoil board and run the adaptive profiling program at full depth (or two passes if 1/4" is too much for your mill).  If you're worried about the extra holes weakening the wrenches, put the holes on little tabs stuck out from the tool profile and you'll cut them off by hand after you machine everything.

Just to put things in perspective, I modeled a quick duplicate of your spanner in Fusion (assuming about 6" long and a 3" hook).  Set it up with a 1/4" 3-flute uncoated end mill.  Max speed of 6k RPM.  Stock was .050" bigger than the max part dimensions.

Time to slot (2D contour at 0.025"DOC) - 1 hour 13 minutes, based on your 3-4 IPM feed.  I assumed you could go greater DOC due to the increased stiffness of the .25" endmill.

Time for 2D adaptive with a cleanup 2D contour finishing pass. (.250" DOC, 15% step-over, 54IPM ).  *9 minutes*.  And only .15 horsepower.

And that's turning everything in to chips - if you hacksaw off most of the stock you can change the CAM setup stock so it only cuts what's really there and cut the time way down.  And if you use the spoil board trick you can set your work origin to one of the holes in the spoilboard and then you don't care if the sawed stock is ragged on the edges.  Just add a bit to the stock in the CAM setup and let it cut air for a pass so you don't bury the tool at 54IPM.

Add 10-15 minutes to drill/tap the stock and spoil board and you're still way ahead.  And the tool lasts longer and less risk of chip welding and tool breakage.


----------



## Wreck™Wreck (Dec 1, 2017)

You did not mention what the aluminum alloy and temper is, if as you say it is from sheet material it may well be 6063 which you will find extremely annoying to work with as it will build up on most tooling. If you can't use heavy flood coolant try coated end mills, there are coatings for just such applications, TiB2 being one, TiN is better then nothing.

Good Luck


----------



## Robert LaLonde (Dec 1, 2017)

ZRN is a decent coating for aluminum, but TiN is in my experience worse than bright.  AlTiN TiAlN and other aluminum nitride coatings are much worse as the aluminum in the coating bonds with the aluminum. If I was going to go with a coating for dry aluminum I'd definitely go with Diamond or ZRN.  

Typically I use bright carbide with flood for aluminum for best overall results.  Even when I have to machine 5052 which is far worse than 6063.  6061 bar and 5052 sheet are the most common alloys at your local metal yards, but yes other stuff is around, and I have no idea what that garbage is they sell at Lowes and Home Depot.


----------



## spumco (Dec 1, 2017)

Bob La Londe said:


> I have no idea what that garbage is they sell at Lowes and Home Depot.



I've PMI'd the crap at Home Depot and Lowes when we had an emergency at work and it's 6061.  No idea of the temper, if any.  Gummy as hell, but it welds about like 'known' 6061-T6.


----------

