[MetalShavings]

I've been using a 1/2" coated carbide four flute end mill to machine some 1018 steel flat bar. Using the speeds and feeds calculators of my NewFangled wizards software I can generally get a decent finish on my parts but recently I've started to question the numbers being output by this Wizards software.

Is there someone here that uses one of the high-end feeds and speeds calculators that can give me the numbers that your software puts out?
As I've stated; I'm using a half-inch carbide four-flute square coated end mill on 1018 cold rolled. I'm machining with my tormach 770. I want to see if my feeds and speeds come anywhere close to the numbers produced by higher end speeds and feeds calculators.

I generally make shallow cuts of .01"-.015" in order to get a finish that doesn't require alot of post-machining work. I'm afraid if I post my present Feeds and Speeds this request for info might take a turn for the worst and go off on different tangents. I'll post my feeds and speeds after I've gotten some relies from some of you high end software users; or, if you have the NewFangled Wizards software you can input my info into the fields and know what I know for now.

After all is said and done, it may turn out that my end mill is just in need of replacing or sharpening. At any rate; it would be nice to know what your software deems as optimum as far as feeds and speeds go. If possible, an optimum depth of cut would be nice too.

MetalShavings

[wtopace]

Since you don't mention the type of coating, I assumed TiAlN. The type and mfg of the endmill makes a HUGE difference in feeds / speeds / surface finish by the way. Cheap chinese end mills have never worked well for me. US made end mills are always worth the extra price they command. I'm actually working now on converting over to variable helix end mills to step up once more.

Best of luck!

EDIT: Btw, you should pick up a copy of HSM Advisor, it's well worth the cost in time and tool savings.

Here's a quick calculation from HSM Advisor (only override is WOC set to 0.015". I have tool stick out set to 1.5", not sure what yours actually is):

Material: 1018 (126 HB)
Tool: 0.500in 4FL Carbide TiAlN Solid End Mill
Speed: 662.0 SFM/ 5059.9
Feed: 0.0039 in/tooth 0.0157 in/rev 79.54 in/min
Chip Thickness: 0.0013 in
Reference Chip load: 0.0026 in
Engagement: DOC1.00 in WOC0.02 in
Effective Dia: 0.500 in
Cross Section: 0.06 x Dia.
Power: 0.6HP
MRR: 1.19 in^3
Torque: 0.66 ft-lb
Max Torque: 7.90 ft-lb
Cutting Force: 31.7 lb
Deflection: 0.0001 in
Max Deflection: 0.0015 in

[Steve Seebold]

The absolute best end mill I have EVER found for putting steel is one made by Dura Mill. It's called Whisper Cut.

It's a 3 flute end mill that comes with a .030 corner radius unless you order is different.

They are a little on the pricey side, but they work really well.

[MetalShavings]

Since you don't mention the type of coating, I assumed TiAlN. The type and mfg of the endmill makes a HUGE difference in feeds / speeds / surface finish by the way. Cheap chinese end mills have never worked well for me. US made end mills are always worth the extra price they command. I'm actually working now on converting over to variable helix end mills to step up once more.

Best of luck!

EDIT: Btw, you should pick up a copy of HSM Advisor, it's well worth the cost in time and tool savings.

Here's a quick calculation from HSM Advisor (only override is WOC set to 0.015". I have tool stick out set to 1.5", not sure what yours actually is):

Material: 1018 (126 HB)
Tool: 0.500in 4FL Carbide TiAlN Solid End Mill
Speed: 662.0 SFM/ 5059.9
Feed: 0.0039 in/tooth 0.0157 in/rev 79.54 in/min
Chip Thickness: 0.0013 in
Reference Chip load: 0.0026 in
Engagement: DOC1.00 in WOC0.02 in
Effective Dia: 0.500 in
Cross Section: 0.06 x Dia.
Power: 0.6HP
MRR: 1.19 in^3
Torque: 0.66 ft-lb
Max Torque: 7.90 ft-lb
Cutting Force: 31.7 lb
Deflection: 0.0001 in
Max Deflection: 0.0015 in

You are correct on the coating assumption. I'm afraid I just forgot to specify the coating type. Also, although they are pricy to me, the carbide end mills I used are not US made. Perhaps that's why they seem to go dull so quickly and not necessarily because of incorrect feeds and speeds.

When I look at the numbers posted here my dyslexia seems to kick in. Just to clarify; the calculated speeds here are 5059.9 and the feeds are 79.54??? If so, I have to think to myself, Holy-Krapp! The feeds and speeds that my wizards calculator is giving me are much slower. Even with shallow depths of cut I was still getting the little circular swirly machining mark finishes. If these posted feeds and speeds are the optimum feeds and speeds I was searching for it's no wonder I wasn't getting the finishes I was hoping for.

On the "Engagement:" line, can you clarity? I'm not sure if the DOC1.00 in is referring to the overhang of my end mill from the holder or something else. "WOC0.02"; is this that actual depth of cut or how does this apply? To me WOC means width-of-cut.

Thanks for your help. I really appreciate it. Over coming these small ignorance problems helps me make big gains in experience.

MetalShavings

[zero_divide]

You are correct on the coating assumption. I'm afraid I just forgot to specify the coating type. Also, although they are pricy to me, the carbide end mills I used are not US made. Perhaps that's why they seem to go dull so quickly and not necessarily because of incorrect feeds and speeds.

When I look at the numbers posted here my dyslexia seems to kick in. Just to clarify; the calculated speeds here are 5059.9 and the feeds are 79.54??? If so, I have to think to myself, Holy-Krapp! The feeds and speeds that my wizards calculator is giving me are much slower. Even with shallow depths of cut I was still getting the little circular swirly machining mark finishes. If these posted feeds and speeds are the optimum feeds and speeds I was searching for it's no wonder I wasn't getting the finishes I was hoping for.

On the "Engagement:" line, can you clarity? I'm not sure if the DOC1.00 in is referring to the overhang of my end mill from the holder or something else. "WOC0.02"; is this that actual depth of cut or how does this apply? To me WOC means width-of-cut.

Thanks for your help. I really appreciate it. Over coming these small ignorance problems helps me make big gains in experience.

MetalShavings

Hi,
"Stickout" is the overhang.
WOC is the actual width of cut.
DOC is the actual depth of cut.

[MetalShavings]

I must be misunderstanding something. I'm having a hard time grasping the DOC being one inch. Does this mean that the software has calculated the optimum depth of cut as being one inch deep per pass? It's hard for me to picture that happening without getting the effect of deliberately crashing my 1/2" carbide end mill into my part. Fortunately I only have to go .27" deep overall but even then, taking that amount of cut per pass seems like it would bog down my little 770 big time. I must be missing something here.

I'd love nothing better than to machine my small parts in one pass of .27" and still get a decent finish to boot. I don't think this little tormach has the balls for that kind of cut and I'm afraid to try that deep of a cut for fear of damaging the mill.

Please correct me if I'm wrong because I really would like to get this particular aspect of this milling job ironed out.

Here's another question; it's about the 1018 metal stock I'm machining. Is this type of steel considered soft, medium or hard within the context of a software such as HSM or the rudimentary wizards software?

MetalShavings

[SCzEngrgGroup]

Those feeds and speeds are assuming you are using HSM (High-Speed Machining) toolpaths, which means constant engagement, with a small width of cut, large depth of cut, and high feedrate. If your CAM is NOT capable of doing HSM toolpaths, you WILL break the tool.

Regards,
Ray L.

[tmarks11]

Think of it this way; you have a bar of a steel 1" thick, and you are using the edge of the end mill, and taking 0.020" off (WOC) each pass. Not that bad (assuming your endmill has at least 1" of cutting length).

This would be like taking a 1" facemill and cutting 0.020" off the surface in a pass (which might sound less extreme, yet requires more HP than the previous edge cut).

No guarantees on the surface finish, but if you take a finishing cut full depth, 0.010", it should neaten things up.

[MetalShavings]

Those feeds and speeds are assuming you are using HSM (High-Speed Machining) toolpaths, which means constant engagement, with a small width of cut, large depth of cut, and high feedrate. If your CAM is NOT capable of doing HSM toolpaths, you WILL break the tool.

Regards,
Ray L.

Ah; that's the information I was missing. I use SprutCam to churn out my tool paths. I don't think it's set up to do HSM tool paths but I could be wrong. Maybe it is; I just don't know how to configure it to output HSM tool paths. I'll have to check on it.

It sounds like HMS machining utilizes the side of the end mill to make the cuts as apposed to the square bottom of the end mill in the manner I'm accustomed to milling.
Thanks for clearing that up. I knew something didn't seem quite right with the DOC listed in the initial reply. I mean, it's perfectly fine for the High Speed Machining it was intended but, if I'd used it for the kind of traditional milling I generally do it might have ended badly for me.

So, HSM machining aside; I'd like to ask my original question again. Assuming that I'm using conventional milling with all the tools and perimeters I've already listed, what would be the optimum or ideal feeds and speeds?

MetalShavings

[SCzEngrgGroup]

Only going 0.015" deep is a verrrrry slow way to go, and you'll end up using up the end of the tool, leaving the sides pristine - not economical.

For 0.015" depth, full-width slotting, HSMAdvisor says 4200 RPM @ 20 IPM. At 0.25" depth, you can go 11 IPM. If you're not slotting, you can go a bit faster.

That said, what's really best for your machine, and your tool, can only be determined by experimentation. Start out conservative (reduce BOTH RPM and feed proportionally), and do a test cut at your desired width and depth of cut. If it cuts well, then crank up BOTH RPM and feed in increments, until it start sounding unhappy, or surface finish suffers. My experience with 1018 is that the quality is all over the place - some of it cuts beautifully, some of it is just cr@p. You must experiment with your machine, your tool, and your metal to find the best parameters. Machine and fixture rigidity will make a HUGE difference.

Regards,
Ray L.

[wtopace]

Those feeds and speeds are assuming you are using HSM (High-Speed Machining) toolpaths, which means constant engagement, with a small width of cut, large depth of cut, and high feedrate. If your CAM is NOT capable of doing HSM toolpaths, you WILL break the tool.

Regards,
Ray L.

Ray - Not trying to start anything, but I'm sorry I would have to disagree. This is from my own personal experience having NEVER broken an end mill with low radial engagement machining ("high speed machining"). Turtle (Large WOC / small DOC) vs rabbit (small WOC / large DOC), I have done both, I much prefer the second and cut my runtimes in half usually... real numbers on my real Tormach 1100 making real steel parts (4140, 1018, 12L14).

Like the OP, I also run Sprutcam and without the magical HSM module. I run "high-speed machining" feed and speeds all the time, especially on steel. No point in wearing out the bottom 0.015" of an end mill and throwing it out 95% brand new. I always choose a deeper DOC and run the tool around the part many times with a thin WOC and large DOC, use as much of the cutting edge of your end mill as you can.

Things to avoid when running "high-speed machining" feeds and speeds (I'm sure there are lots more):
1) Avoid slotting - trochoidal tool paths if you have to slot
2) Avoid plunging - always helical ramp, 2-5 degrees slope angle works well
3) If you get chatter, reduce the DOC or make your setup more rigid
4) ALWAYS set your feed rate DROs to ~25% on the first run, bump it up as you feel more comfortable, 100% is usually the quietest and smoothest running
5) Leave about 0.010" for a slower (half the feed rate is usually what I start with) cleanup pass.
6) Enjoy the fact that your mill isn't going 10 IPM loudly pounding, but instead blazing at 60-70 IPM with a nice whizz sound and long thing chips instead of short fat chips.
10) I have never broken a tool with "HSM" feeds and speeds and this process

Also remember that a thin chip (shallow WOC) also means you're only using the very outer radius of the end mill, so chip thinning applies. You'll need to INCREASE your movement speed to keep the same chip you would get from a slower IPM with a larger WOC engagement. You may think 70 IPM sounds crazy, but it's in reality, it's not that bad.

To the OP - Find what works for YOU =) You will be surprised at what the Tormach 1100 can do, I sure was once I got away from my RF45 style of machining. Don't be afraid to push your machine, tools are a lot stronger than we think and I really only break them from true crashes, not from actual cutting (my machine will bog long before my tool breaks).

Best of luck!

[popspipes]

Ah; that's the information I was missing. I use SprutCam to churn out my tool paths. I don't think it's set up to do HSM tool paths but I could be wrong. Maybe it is; I just don't know how to configure it to output HSM tool paths. I'll have to check on it.

It sounds like HMS machining utilizes the side of the end mill to make the cuts as apposed to the square bottom of the end mill in the manner I'm accustomed to milling.
Thanks for clearing that up. I knew something didn't seem quite right with the DOC listed in the initial reply. I mean, it's perfectly fine for the High Speed Machining it was intended but, if I'd used it for the kind of traditional milling I generally do it might have ended badly for me.

So, HSM machining aside; I'd like to ask my original question again. Assuming that I'm using conventional milling with all the tools and perimeters I've already listed, what would be the optimum or ideal feeds and speeds?

MetalShavings

I use an old version, Sprut 7, there is a selection in the hole pocketing op that is called HSM I dont really know if this is what youre referring to, I have never used it myself. The newer versions of Sprut most likely have this option as well.

Attachment 296338

[hanermo]

An observation of the calcs.

HP used is only 0.6 Hp, and cutting force was 32 lbs.
These are not big values, and should work fine on many machines.

[wtopace]

I use an old version, Sprut 7, there is a selection in the hole pocketing op that is called HSM I dont really know if this is what youre referring to, I have never used it myself. The newer versions of Sprut most likely have this option as well.

Attachment 296338

That selection will generate trochoidal tool paths (small circles instead of slotting). I always run these types of paths, as they seem better all around to me, so no reason to risk breaking a tool in a slot. With the same speeds and feeds, however, it will usually increase run time (higher speeds and feeds can be run with this selection though).

The HSM module is actually an add-on that goes under "Machining Strategy" section (See screenshot below). This module attempts to keep a constant chip load, as Ray mentioned above. Of course, with ANY machining operation, a constant chip load is ideal, but unfortunately it is never possible due to entry / exit. This module and HSM Works (Fusion 360 CAM) attempts to gradually increase chip load on entry and gradually decrease chipload on exit, while maintaining it during profiling... all great things.

What you really don't want is your tool slamming into metal with a large WOC at a high feed rate - regardless of whether it is intentionally programmed or not - I would call this a crash =) This is what breaks tools. I cannot imagine breaking a tool with a 0.015" WOC at any feed rate a Tormach is capable of.

Attachment 296340
NOTE: These are all default values and not recommended settings for any real machining op

[MetalShavings]

I know that the answer I'm looking for in somewhere within the latest replies I've gotten. My version of SprutCam does have the features that a couple of you guys have mentioned. I just have to learn how to use them. I guess that from here, I'm off to YouTube in search of tutorials showing me how to do HSM stuff using a tormach and SprutCam.

Many thanks to all of you guys who took the time to reply to my inquiry. You guys never let me down when I need help.

Tim M.

MetalShavings

[wtopace]

Don't be afraid to try the new ways of machining, you'll probably be pleasantly surprised. Next time you buy end mills, pick up a few spares and set them aside as, "I don't care if I break them, these are my try-new-things end mills", it will make life easier being prepared to move out of your comfort zone =)

[SCzEngrgGroup]

Ray - Not trying to start anything, but I'm sorry I would have to disagree. This is from my own personal experience having NEVER broken an end mill with low radial engagement machining ("high speed machining"). Turtle (Large WOC / small DOC) vs rabbit (small WOC / large DOC), I have done both, I much prefer the second and cut my runtimes in half usually... real numbers on my real Tormach 1100 making real steel parts (4140, 1018, 12L14).

I don't think you're really disagreeing. It all comes down to the toolpaths the CAM generates. Since you apparently CAN do helical entries, trochoidal paths, an the other things you mention (which are all part of HSM), you are, in effect, generating HSM toolpaths, even if it's not called that explicitly. There are many CAMs out there that cannot do those things, and can only slot by doing a plunge, followed by a horizontal feed. And, they will generate toolpaths with widely varying width of cut, loading the tool very heavily in corners, for example. If your CAM allows you to limit maximum width of cut, as yours apparently does, you'll be fine. But many CAMs do not provide that ability. For example, some of the low-cost CAMs which are very popular among hobby users will always starts a pocket with a slot, then will start doing peripheral milling outward from that slot, yet you only get to specify a single feedrate for the entire operation. If you use that CAM, and program in a 1" DOC and 0.015" WOC at 60 IPM, you'll get about 0.010" into the slot before the tool breaks.

Regards,
Ray L.

[wtopace]

I don't think you're really disagreeing. It all comes down to the toolpaths the CAM generates. Since you apparently CAN do helical entries, trochoidal paths, an the other things you mention (which are all part of HSM), you are, in effect, generating HSM toolpaths, even if it's not called that explicitly. There are many CAMs out there that cannot do those things, and can only slot by doing a plunge, followed by a horizontal feed. And, they will generate toolpaths with widely varying width of cut, loading the tool very heavily in corners, for example. If your CAM allows you to limit maximum width of cut, as yours apparently does, you'll be fine. But many CAMs do not provide that ability. For example, some of the low-cost CAMs which are very popular among hobby users will always starts a pocket with a slot, then will start doing peripheral milling outward from that slot, yet you only get to specify a single feedrate for the entire operation. If you use that CAM, and program in a 1" DOC and 0.015" WOC at 60 IPM, you'll get about 0.010" into the slot before the tool breaks.

Regards,
Ray L.

Gotcha - Guess I have never used a CAM that would disregard my WOC setting of 0.015" and decide to slot... but it makes sense they are out there. Sprutcam may be difficult to learn, but it is extremely powerful once the tricks are mastered. I'm working on becoming as proficient in Fusion360 CAM as well, but it's quite different from Sprutcam, so I'm having to relearn all of my tricks.

Now that Fusion360 is so cheap / free (depending on your business or hobby needs), I recommend it all the time people who are in need of a CAM tool or upgrade.

[pickled]

I guess that from here, I'm off to YouTube in search of tutorials showing me how to do HSM stuff using a tormach and SprutCam.

MetalShavings

Here you can see trochoidal entry and some constant engagement trochoidal vs. slotting. Learning is fun, but painful at the same time.
https://youtu.be/E1QxiuriR6I

[MetalShavings]

Yea; I'll probably give HSM a try. I have about 3 different 1/2" carbide end mills I can afford to break right now. They're the same ones that had started to give me less than ideal finishes using them to do conventional style milling. The bottom faces may be slightly dull but the side cutting faces are nearly pristine.

My problem now is figuring out exactly which features to use and how to input the numbers in my SprutCam software to output some usable HSM tool paths. It will be like learning SprutCam all over again. Even when using it to do conventional milling, I never could figure out how to get my end mills to angle into my work piece gently from the side rather than plunging in from the top.

It's that SprutCam learning curve that's a killer.

MetalShavings