# A36 Steel.   New Mill 1st Cuts.  Hss? Carbide?



## countryguy (Apr 6, 2015)

OK, so the new Mill is cutting plant foam really nice...time to Graduate and I'm getting cold feet.  

The Mill: 2HP SuperMax YMC 30 taper.  
The Part:  A 6+ inch mold pattern the son needs for an Axe project.   .125 total depth on two pockets.  (2 passes for .125 )  Then a 'merge' or taper edge all the way around the larger pocket.  (images below). 

I was told that A36 was equiv to 1020 but that's not what I'm reading online?? Some say closer to 1030??   Here is my short list of Q's: 

1) I bought HSS cutters for this and now wonder if I should break out the Carbides?  I do not want to waste 2 or 3 endmills only to find out I need the Carbides.  
2) With HSS end mills do you usually cut w/ Mist or air on part.  I do not have the flood up yet. 
3) Using GWizard  HSS 5/8 end mill = IPt .003 , RPM 978 and Feed IPM of 15.57
4) Using  GWizard: Carbide/Coated . IPT  .0027  RPM 2892 Feed IPM of 40.87 (seems really fast!)

Just don't know the materials all that well yet!  Appreciate any comment or suggestions.     This is just some test stuff we wanted to do.


----------



## JimDawson (Apr 6, 2015)

A36 machines OK, it's a little gummy.  I would probably start with a cobalt rougher and reduce the feed to about 5 IPM and the RPM to about 600.  Then run a finishing pass with a 4 flute at about the same feed and speed.  I use a mist system on both HSS and Carbide.  The only time I use just air is on tool steels.  I generally run a bit slower than optimum speeds, no point in beating up the tooling and machine if you don't have to.  I'm normally not in that big of a hurry.

The GWizard assumes a full blown production environment with optimized tooling and coolant.


----------



## markknx (Apr 6, 2015)

Can't help on the feed as I do that by feel. I agree with Jim but would add Cut lots A36 (get for free from work)   HSS will cut it fine and hold up good.  Save the carbide for good steel. keep the chips out of the way because as mentioned by Jim A36 is gummy  if you start re cutting them (Like in a pocket) they will gall the cutter and give a poor finish.


----------



## countryguy (Apr 6, 2015)

Ok, Horse stalls are all plowed out for Spring....  My afternoon is now setting up for  .625 @  IPT .002 (in range),  an RPM of 575 on Coolant Air Mister and some crossed fingers.    I know I need to just get in there!  Thanks everyone! 
JJ   




JimDawson said:


> A36 machines OK, it's a little gummy.  I would probably start with a cobalt rougher and reduce the feed to about 5 IPM and the RPM to about 600.  Then run a finishing pass with a 4 flute at about the same feed and speed.  I use a mist system on both HSS and Carbide.  The only time I use just air is on tool steels.  I generally run a bit slower than optimum speeds, no point in beating up the tooling and machine if you don't have to.  I'm normally not in that big of a hurry.
> 
> The GWizard assumes a full blown production environment with optimized tooling and coolant.


----------



## countryguy (Apr 7, 2015)

Dear Diary, ohh horse pucks.    Did not get to run my 1st CNC job yesterday.   Came so close.   but realized I did NOT: 
- Put in a 0,0 mark where I could place the endmill to insure my part is cut where I want it.  
- Did not have my 5/8 hold down kit and t-nuts.  (Came UPS 4pm.. the gods do love me!).
- The cut setup I had for the "chamfer" was all wrong.  Had to redo the entire program.  (Manual milling sounds better all the time). 
- The Boss called me to the barn . (wife I adore ;-)   Noithing went right yesterday! 

- Today,  I have the plate sitting on the mill, Program all cleaned up, Ran a test 3" above the steel and just watched it go round & round to make 
sure my bolt-down/hold-downs would be clear.   And yep.... I think we're about ready to green light this after a refreshing cup O'joe. 

My point is that I often see folks comment that they could have milled 3 of what-ever manually -vs- CNC and all the work ya do on the front end. ;-)   But I think I like it?  Looking to do more manually for sure in the coming months.  

Being a rookie here w/ you guy's is very comforting!  Thanks for ALL THE HELP to get us this far.   To Jim D.   I think the kid and I would be lost w/o ya! 

Time to put this to bed. 
CGout.


----------



## Wreck™Wreck (Apr 7, 2015)

countryguy said:


> OK, so the new Mill is cutting plant foam really nice...time to Graduate and I'm getting cold feet.
> 
> 3) Using GWizard  HSS 5/8 end mill = IPt .003 , RPM 978 and Feed IPM of 15.57
> 4) Using  GWizard: Carbide/Coated . IPT  .0027  RPM 2892 Feed IPM of 40.87 (seems really fast!)
> ...


Is this a knee mill? If so the S&F's are a bit aggressive I imagine (-: 
Without a good amount of high pressure flood coolant I wouldn't even try that, you will be recutting the chips over and over again in the pocket.


----------



## countryguy (Apr 7, 2015)

Could you share some insight on DOC and WOC values and SFm's you'd suggest?  The Carbide's are way too fast.... I agree.  Jim's suggested feed of 5 and rpm 500-600ish.   But I've been wondering how much to bite on the width and depth.  I now have .06 depth and width's stacked up to reach my target depth of .125    I mean all this to get and 1/8th into the metal is a 3hr. CNC run w/ these feeds and speeds.    sound about right?


----------



## JimDawson (Apr 7, 2015)

I think you would be safe with a 0.4 stepover, and a 0.120 DOC, leaving 0.005 for a finish pass if you want, or just go for the full depth if the finish is not critical.  Your machine is about the same size as mine so I'm pretty sure it will take a lot more than that.

Here is a picture of a 0.500 rougher plowing through 7/8 inch A36 @ 0.5 IPM at about 600 RPM




And the same rougher plowing through 1/2 1018 @ 3IPM  This started as one solid plate, I did it in 2 passes, one roughing pass at full depth, and a 0.015 finish pass with a 2 flute.  I should have used a 4 flute for the finish pass, but I didn't have a sharp one.


----------



## countryguy (Apr 7, 2015)

Jim,  When I grow up I hope to be as good as you       I need a rougher!   Going on Amazon tonight.  Which brand do you like?  HSS coated or plain?   TIA! 

Those are numbers I would expect as it's why I bought the 30taper and a 3000Lb Mill.  
Jeff.


----------



## JimDawson (Apr 7, 2015)

I'm not good, just lucky sometimes.  I also never professed to be a machinist, I'm just a problem solver who happens to need to use machine tools sometimes.

I normally buy Interstate from Enco.  Hertel is a higher end cutter, Enco sells both, but I haven't noticed a real difference in quality.   There are fine roughers, course roughers, finishing roughers (now that's an oxymoron), uncoated roughers, coated roughers, coated in TiN, TiCN, Tialn, Bright

It really depends on the material and the job.  Enco has pretty good explanation of the different roughers and their uses.  I normally buy 2 to 5 at a time depending on how low my stock is, this is true for any cutters I buy.  It really sucks to be in the middle of a job and break or wear out a cutter and not have a replacement to finish.


----------



## markknx (Apr 7, 2015)

I never place an order without adding a couple of cutters, I check to see what I have the least of or want to add. And I have a small machine if I had a big machine I would need even more cutters.
Jim I'm with you on the Machinist thing. I'm more of a hog it out till it works guy. well maybe not that bad.
Mark


----------



## countryguy (Apr 8, 2015)

I much prefer Electron flow personally, but this is such a fun hobby/craft that to learn!   Thanks all.   I bought some chip breakers from Melin/Amazon.  US based and US owned and Operated.  Trying to always buy US when I can.  then someone miss keyed a price on 3/4 coated CB type for $15 on Amazon....(I think they should be $51)  I bought 2 of the 3 in stock    And the 5/8" for $37.    

Will still plan on trying a single area clear of 3 today w/ this 4 flute un-coated.


----------



## Wreck™Wreck (Apr 8, 2015)

countryguy said:


> Could you share some insight on DOC and WOC values and SFm's you'd suggest ?


Not enough info supplied on your machining conditions and machine or the size of the part.

Start with a low feed rate and if it runs well start bumping up the feed overide, if the spindle speed seems off, wait until it is in a non cutting move and feed hold it then adjust the speed.


----------



## countryguy (Apr 9, 2015)

That was easy enough!  The 30taper is a Huge improvement over the hobby mill.    I did take the full .125 depth and a .15 cutover (if I recall)... That was like popping thru butter as someone noted.  Chips coming off were fine on 581 RPM and 5.5IPM 95SFM and .0024 IPT.   Nice!!!!  Could easily take more but it's' our maiden voyage!    Here's a video!   



        I get what 'hoggin' feels like now.  LOL.  

I wonder how well she'll do w/ 1045 steel and the kids axe cuts?


----------



## JimDawson (Apr 9, 2015)

Your video is set to private, so we can't see it.


----------



## countryguy (Apr 9, 2015)

Sorry.  I'm not on usually. I set it to unlisted now.  Should work.  



JimDawson said:


> Your video is set to private, so we can't see it.


----------



## JimDawson (Apr 9, 2015)

That's cool!  Looks like it works.  That's a pretty stable machine, it will make piles of chips in a hurry.


----------



## countryguy (Apr 9, 2015)

I pulled out the Rougher to see what it looked like.  This anything to worry about?  It obviously mushed over swarf and packed it into the non-center cutting middle.


----------



## countryguy (Apr 9, 2015)

I was able to pop it all out w/ a small pointed awl type tip.   ;-)    Sorry to keep dragging this post on and on, but it's all about learning and learning and then teaching and Mentoring.  ;-)


----------



## JimDawson (Apr 9, 2015)

countryguy said:


> I am not able to pop it out at all.  bummer... did I ruin a less than 12hour old endMill?  ;-(



I think the problem is that you were plunging with a non-centercutting end mill, and a lack of coolant. 

There are three ways around this.

One of course is to use a centercutting end mill, but end mills really don't like to be drill bits, they tend to walk a bit.

Another is to use a 15 degree lead-in move on the cut, ramp the Z-cut down into the work as the X/Y is moving, thus the end mill is not plunging straight down. This is normally an option in the CAD software.

One of my favorite tricks is to drill a hole at the plunge point almost to the target depth, using a drill or a center cutting 2-flute end mill.

A mist coolant system will be helpful also.


----------

