Small Miill Drill - Hard Milling, 1045, and DOC/WOC advice from ya'll

[countryguy]

Hi everyone, As many know my Son and I are total newbies on the Milling /CAM/CNC side. Came over from Plasma & 2.5 work.
What we have : My kid and I have a 3:1 combo 2hp Mill Drill Lathe setup.
What we are machining: 1045 steel (small pics attached) w/ only small workloads (or so I thought).
cutter= IMCO 525 5/8 and a 1/2 combo rougher/Finish Both tried w/ maybe moderate success.

Here is the issue: (remember, it's only been about 1 month on our OJT here. ;-) I keep chipping the corners off my end mills. chatter and vibration seem abundant. I simply cannot continue to experiment upon this level of steel hardness and ruin pricey hard steel cutters. The Son is young and thinks this will work. I'm starting to think we should go mild steel and try to harden post milling? He is trying to start his own business so I'm trying not to discourage him into a different product just yet. (he's 17).

I'm reading and experimenting about harder steel milling and wanted to ask something. Are Mill cuts in the .02-.05 WOC/DOC range seemingly OK if that's what it takes? It seems to me that I should be able to get some better cutting than this? Feedrate is 5 to 8 and far from the GWizard and Imco specs in the 20's and 30's. chip-loads in the .0012 range. (should be high 20's / low 30's). but I keep the SFM dialed as best I can.

Specs: I have the RPM to 1100-1300 w/ 1/3-1/2 chiploads as a full chip-load seems to chatter like crazy. Width is usually just a .04-.07 step-over. Depth of cutter is about .06 tops. This seems to allow me to get thru the material albeit really slow. I now started to setup DolphinCam to just go around 2x or 3x to get me into the -.1 depth range w/ .03 depth passes. that's 1hour-30mins to mill out 1 axe face side.

What is My question: Does this seem like we're on track with this? All we are doing is a Z ramp cut from -0.00 down to -.09-.1 in multiple passes. To me it seems like the corners are taking a beating while ramping down into material and maybe passing a tiny tiny load onto the flute sides (my assumption here). I tried a ball mill just to compare and it tore the cutter head clean off when it hit face edges. Bad idea.... Not sure a Corner radius would help? Just a blunted corner slamming into the edges as it slopes down in. Maybe a grinder would be easier, but hey - We're having fun together and that counts for a bunch!

Anyone like the insert style cutters? Maybe he would have better luck and predictability of cut parms with those? I cannot find too many articles or suggestions for plasma cut 1045 w/ lower end hobby mills. ....And I'm starting to see why.

 

[xalky]

I would definitely harden the material after all the machining is done, even roughing in your cutting edges prior to grinding. You can grind your cutting edges after its hardened. Try using some smaller 3/8 " roughing cutters to minimize chatter. Carbide cutters will last much longer, but practice with hss cutters first.

Sent from my SPH-L710 using Tapatalk

 

[countryguy]

Thanks for the notes! What hooked me on using 1045 up front was the industry OEMs push this marketing info noting these crazy depths and SFM /feedrates and how invincible their cutters are on the hardest of hard materials. I also had assumed that the larger the cutter, the stronger my Corners would hold up? Somewhere I read that using the largest size cutter for a job is the 1st approach to take? Will run a 3/8 in next then.

...I am but the sum of my mistakes generally.
CG out for today.

I would definitely harden the material after all the machining is done, even roughing in your cutting edges prior to grinding. You can grind your cutting edges after its hardened. Try using some smaller 3/8 " roughing cutters to minimize chatter. Carbide cutters will last much longer, but practice with hss cutters first.

Sent from my SPH-L710 using Tapatalk

 

[xalky]

Thanks for the notes! What hooked me on using 1045 up front was the industry OEMs push this marketing info noting these crazy depths and SFM /feedrates and how invincible their cutters are on the hardest of hard materials. I also had assumed that the larger the cutter, the stronger my Corners would hold up? Somewhere I read that using the largest size cutter for a job is the 1st approach to take? Will run a 3/8 in next then.

...I am but the sum of my mistakes generally.
CG out for today.

The biggest part of your dilemna is the the lack of rigidity of your machine. A smaller cutter will cut down the lateral forces that are encountered, which are causing the chatter. You wouldn't experience these problems with a big heavy rigid machine. A softer material will also lessen the chatter. Do both and you should see much better results.

 

[JimDawson]

I think I see a few issues here. The cutting milling speed for annealed 1045 using HHS endmills is about 50 to 75 FPM, so for a 1/2 inch endmill that would be about 400 to 600 RPM. With a cobalt rougher you might bump that up a bit. I suspect the edge of the work is still a bit hard so you might want to be on the lower end of the range.

On your machine a feed 5 to 8 IPM seems reasonable, like xalky stated, your machine is not ridged enough to take much more. A roughing endmill likes a little less feed, but will take more depth of cut. In hardenable material you do need to maintain enough feed to keep the tool from rubbing and thus keep the material from work hardening. You could try bumping up the feed speed a little. Normally I will start out a a lower feed speed, and then bring it up until I find where the machine is happy without being overloaded. On my machine, sometimes I bury a 1/2 inch rougher 3/4 inch deep in mild steel and take a full endmill diameter cut for profiling.

I would also start at the outside of the work and move the z axis up to cut the shape, rather than plunge, especially when using a roughing endmill. I would use a stepover of about Dia x 0.4, a 0.06 DOC seems OK. If you can run your machine manually with hand wheels, I would play with the feed and DOC to see how the machine feels, you can feel it when the machine is starting to overload.

I'm also guessing the you are getting more chatter on the second side of the work. It's pretty easy to clamp down the flat plate to get support under the work area. On the other side, it is more difficult to support the work area due to the angle already machined. I would build some wedges that can be placed under the finished side to give better support.

If you can tilt your head, and have enough travel, you might be able to use a flycutter with a carbide tool bit, or a large carbide insert facemill and mill it in about 3 or 4 passes. I think you have enough horsepower to do this, but there a question about rigidity.

Most of all, have fun with you son. That may be the most important part of the whole operation.

 

[Ray C]

Agreed with all that's been said...

Also, do note, 1045 will work harden very quickly and when it does, it will beat-up carbide quickly and will eat HSS like popcorn. Don't play games with soft (annealed) 1045. Make a decisive cut with the proper feeds and speeds -get in and out quickly. Teasing annealed 1045 with light DOCs, excessive RPMs and slow feed-rates is the perfect storm for localized hardening. I've fallen for this trap many times. Any metal above Rockwell 45 is tough on carbide. 1045 will easily go up to Rockwell 55. The hardening will be localized at the area of intended stock removal.

If you wish to machine metal that's already above RC 45 your two best choices are to anneal it down to a softer state or, use ceramic inserts (very risky and fire-hazard prone). Grinding is another option but not usually feasible for stock removal.

The reason GWizard is giving you "unusual" feeds & speeds is because it's giving you what's called "Hard Machining" values. "Hard Machining" is when you take very light cuts but at high RPM rates but also at VERY fast feed-rates. That combination/recipe will not give rise to localized hardening. Those procedures are often used for titanium and Inconel -which are notorious for work hardening... You will not (likely) be able to do "Hard Machining" with any machine costing under 50 grand and/or weighing less than a couple tons -and I dare say, that would be at the very low end of machine capability.


Ray

 

[Ray C]

One additional note: "Hard Machining" is usually done with nitrogen cryogenic cooling nozzles aimed directly at the piece being machined and at the cutter. The cutters used are likely pretty high-end and designed for those applications. I believe a company called Greanleaf has a line cryogenic-use cutters. I use their ceramic inserts and like them a lot.

FWIW, when I cut hardened metals with TiALN carbide cutters, I pay close attention to the mist cooler to make sure it's operating and covering workpiece lead, bit and post-cut area of the workpiece.


Ray

 

[countryguy]

Thanks a TON guys. Your comments are really helpful! Again, THANKS!

I found out the Sandvik Coromant sales office is just a local hop 20mins away from me. I like what I'm reading on this CoroMill 300.... Light cuts, low forces, smooth operation.... Again, all the right buzz words. (link below).

I am willing to pay for an insert based cutter if it works in our application. Nobody seems to allow you to return these tools. Once you use it, you own it. I'm asking Sandvik if they allow a loan/sample or rep visit to see how well it will work? Why not.... I'll spring for Lunch too if he/she comes along.

https://www.sandvik.coromant.com/en-us/products/coromill_300/pages/default.aspx

- - - Updated - - -

Ray, Quick Q if I may? How rigid is the PM45-CNC platform? My Mill is in need of "rigidization". That will be the quest for the next few days. LOVE that Plasma cutter. Braces, mounts, struts in 10-20mins. w/ holes to boot. I guess we found Plasma so fun and easy to do that Milling seemed to be a logical progression.

One additional note: "Hard Machining" is usually done with nitrogen cryogenic cooling nozzles aimed directly at the piece being machined and at the cutter. The cutters used are likely pretty high-end and designed for those applications. I believe a company called Greanleaf has a line cryogenic-use cutters. I use their ceramic inserts and like them a lot.

FWIW, when I cut hardened metals with TiALN carbide cutters, I pay close attention to the mist cooler to make sure it's operating and covering workpiece lead, bit and post-cut area of the workpiece.


Ray

- - - Updated - - -


Ray, Quick Q if I may? How rigid is the PM45-CNC platform? My Mill is in need of "rigidization". That will be the quest for the next few days. LOVE that Plasma cutter. Braces, mounts, struts in 10-20mins. w/ holes to boot. I guess we found Plasma so fun and easy to do that Milling seemed to be a logical progression.

One additional note: "Hard Machining" is usually done with nitrogen cryogenic cooling nozzles aimed directly at the piece being machined and at the cutter. The cutters used are likely pretty high-end and designed for those applications. I believe a company called Greanleaf has a line cryogenic-use cutters. I use their ceramic inserts and like them a lot.

FWIW, when I cut hardened metals with TiALN carbide cutters, I pay close attention to the mist cooler to make sure it's operating and covering workpiece lead, bit and post-cut area of the workpiece.


Ray

 

[DMS]

If you have not seen "Knifemaking Tuesdays" On Youtube, there may be some good stuff there for you. The guys is a custom knifemaker, and has been doing all of his finish work in the hard state (blades are in the high 50s/low 60s RC). It is tricky, and many things seem counter-intuitive. I have not done any hard milling, but have done some hard turning on ballscrews as an experiment.

I am a bit suspicious of the fact you snapped a ball mill on contact. I think that would indicate a problem with the code. Generally radius endmills are tougher than square end mills, and ball end mills are tougher than that.

Regarding moving to larger endmills. That is mostly a fix for rigidity/end-mill flex issues. Like Marcel said, with a smaller machine, you are just not going to be able to push larger cutter hard enough. 2hp seems like a decent sized machine though, so I am guessing it's a bit larger than an X2.

Given the issues you are having, I would suggest looking over the GCode, I have a feeling you are entering the material too abruptly, and that is causing the damage to the endmills.

 

[Ray C]

Thanks a TON guys. Your comments are really helpful! Again, THANKS!

I found out the Sandvik Coromant sales office is just a local hop 20mins away from me. I like what I'm reading on this CoroMill 300.... Light cuts, low forces, smooth operation.... Again, all the right buzz words. (link below).

I am willing to pay for an insert based cutter if it works in our application. Nobody seems to allow you to return these tools. Once you use it, you own it. I'm asking Sandvik if they allow a loan/sample or rep visit to see how well it will work? Why not.... I'll spring for Lunch too if he/she comes along.

https://www.sandvik.coromant.com/en-us/products/coromill_300/pages/default.aspx


- - - Updated - - -

Ray, Quick Q if I may? How rigid is the PM45-CNC platform? My Mill is in need of "rigidization". That will be the quest for the next few days. LOVE that Plasma cutter. Braces, mounts, struts in 10-20mins. w/ holes to boot. I guess we found Plasma so fun and easy to do that Milling seemed to be a logical progression.

CG,

You can get this cutter (or ones like it with round inserts) at Shars.com for about $50-70 bucks. Make sure to get ones with a shank size compatible with your mill. I usually go with 3/4" shanks and I have some with dedicated R8. Keep in mind, you can't do hogging with face cutters like these. When you see the YouTube videos of a machine creating deep paths of perfect cuts, do realize they're using 25+ horsepower machines. Also, the wider the face cutter, the more it will expose your machine's rigidity weakness.

For what I think you want to do, I'd be inclined to try a 7/16, short flute, face cutting, TiALN roughing endmill (as shown).

As far as the PM45-CNC is concerned... It's more than adequate to work on any fully annealed metal or those with Rockwell hardness up to (about) RC 38. For annealed carbon steels, typical cutting parameters with a 3/8" roughing endmill would be about 2600 RPM with feeds ranging between 12 and 25 ipm. The 12 would correspond to a full width cut at 0.1" deep and 25 would correspond to a 0.1" depth side cut with 25% hill climb walk over.

Speaking very honestly... I would not want to sell someone a piece of equipment on a guess it will solve one particular problem such as what you face. The PM45-CNC is not suitable for true "hard machining". I use it a lot and my CAM program calculates feeds & speed based on HSM (high speed machining) rates and from there, I tweak the parameters downward about 30%. Given this, I guess you can classify it as a 70% HSM capable machine.

FWIW, the piece shown in my hand is 3/4" 1050 hot-rolled plate (as-is hardness, probably 125 Br) and the PM45-CNC mill did it in 35 minutes. I was careful with setup and devised (to the best of my ability) intelligent tool paths optimized for dimensional precision. The tolerances all came out to +/- 0.00075 meaning, all dimensions were inside 0.0015" of the target size. For the most part, everything was within a thou. The holes are amazingly round and the only place I hit 1.5 thou tolerance was a tiny spot at the entry point of the holes. I used a circular entry but accidentally used a vertical lead-out. It was the first run part, I'm happy with the outcome -but after watching it cut, I think I could cut 5-6 minutes off the production time. I'm not going to bother to do that optimization; it's not a critical part.

Ray