Here are the images of the test runs I did in both the 303 stainless steel and the 1018 steel. On the stainless steel I have to mention that I was milling a piece 1 1/2" diameter round bar. I don't think this should make any difference here. Once I had milled it flat, my tool path would have then continued on to shape the remainder of the surface. After which, I would have turned the metal stock around and proceeded to machine the top face in the same manner. Incidently; when I milled the 1018 steel test part, I did use some of the suggestions you made in the YouTube video you had posted using the IGES file I sent you. It was really helpful in this instance. Particularly when setting up to mill those very small pockets on the top surface of this part. Tim M.

Broken End Mill on Stainless Closeup Of Bad Cuts On Stainless

I machined my first functional prototype Charge-Handle on Saturday morning. I used my last piece of scrape 1018 steel. Drawing on the experience gained from my first attempt, I tweaked the dimensions of this latest Charge-Handle component and it turned out very functional but still in need of a few more minor tweaks to get it to the overall finished dimensions I'm wanting to attain. I tried to tune my HSM numbers to the exact DOCs with each operation or tool path. The deepest or most material I had to remove in any given operation was only .26" deep so I used the "Speed" recipe that I got from the HSMAdvisor software but I knew from my previous test runs that the WOCs were far to aggressive for my machine. With 1018 steel, the one horse power motor starts to bog down if I cut any deeper than .015" using the 5070-RPMs and the 22.12-Feed that the HSMA software calculated out as "Optimum." Even though I got it to work, I still feel like there is something I MAY be doing that I shouldn't be doing or something that I'm NOT doing that I should be doing because it took nearly as long to finish this prototype using HSM as it would have if I'd done it with conventional milling. It was a little quicker but not as quick as I envisioned. The funny thing was that I checked the recipe I got from HSMA against the recipe I got from FSWizard and found that I was getting way higher feeds and speeds from FSWizard. If I remember correctly, FSWizard was giving me something like 7674-Speeds with one-hundered-plus Feeds with the same numbers I entered in the HSMA text fields; and this -according the the FSWizard software-only required less than half a horse-power. If I ever do another one of these Charge-Handle components in 1018 steel, I think I'm going to try using the higher numbers that the FSWizard software churned out just to see what kind of strain it puts on my Tormach 770 and the half-inch end mill I'm using. One of the errors made by me was in trying to cut this part's thickness to it's exact dimension. I should have left a little more meat on that bone so that when I did my post-maching clean up I'd end up with the correct overall dimensions on the thickness of my part. Oh well; live and learn. After final filing and clean up it worked just as I'd hoped. I fitted the part into the receiver of my rifle and cycled the action a few time. I'm happy with the results. Now on to trying to mill this same part with the 303 Stainless Steel metal stock I purchased earlier. After a few more minor tweaks to my CAD and CAM files I'll be ready to attempt that milling operation. Actually it's going to be split into four separate operations followed by some post-machining work. This time I'll allow a bit more thickness so that I can polish it up to the exact size. I'll post a couple more pictures of the finished parts once I've edited them for clarity. After that you most likely won't hear to much from me about the HSMAdvisor software. I still haven't gotten the hang of this software but I think I'm moving in the right direction. Tim M.

I was laying in bed last night wondering if there was anything I could do to lessen the learning curve and mitigate the tool breakage or potential damage to my Tormach 770 CNC mill while being able to confidently rely on the recipes calculated by the HSMAdvisor software. As it is now, generally speaking; any guy or gal with an under powered hobby mill has to decide weather to take the chance of using the calculated feeds and speeds recipes and risk breaking their cutting tools or subjecting their mills to bogging down to a stand still which will most likely affect accuracy if done repeatedly. I was wondering, rather than risking damage to one's machine, cutting tools or the parts we're trying to fabricate. Is it possible for the end user to change the horse power rating within the HSMA software of their specific machine? In my case, I believe it would be beneficial to use a horse power rating of a 3/4-horse power motor rather than the one-horse-power motor that it is technically rated at. If this can be done, would it cause the software to calculate speeds and feeds based on the smaller horse power and thus calculate recipes that were not so aggressive? For a 1 horse power machine it would be better to assign it a 3/4 horse power rating. A 3/4 horse power rated hobby mill could be assigned 1/2 horse power rating and so on; possibly even assigning a lesser horse power rating depending on the ability of the machine. All other attributes of the mill in question could remain the same, it's just the power rating that would be lessened or adjusted. The one horse power rating of my Tormach 770 is in fact just one horse power. If this one horse power motor is free standing and plugged into an electrical socket, it will spin with the power of one horse power as technically specified. However, when you factor in the drain on that horse power caused by spinning the spindle, turning the tool as it cuts into the part and other factors, That one horse power quickly becomes far less than one horse power. A loose analogy would be a 4 cylinder engine powering a compact car. This engine is rated at a certain horse power but when you figure that this engine is not just free-turing. It also has to turn the pulley for the power-brakes, the fuel-pump, the generator/alternator, the air conditioner and the transmission. All of this things siphon away horse power before it ever turns the wheels of the car to move it along so, the originally specified horse power of that 4 cylinder engine becomes substantially less than specified in the first place. The same holds true in CNC hobby mills of one horse power or less. So again, I was wondering if or when I decide to buy the HSMAdvisor software, would it be possible for me as the end user to change the horse power rating of my ONE-Horse-Power motor down to 3/4 Horse-Power; or, is this something that would have to be done on the programming end of this software? I speak only for myself here. I would much rather use an HSMA calculated recipe that is initially a little less aggressive and work my way UP to the "Optimum" feeds and speeds so as not to stress out about breakages or undue wear and tear on my mill, rather than using a calculated feeds and speeds recipe that is generally to aggressive for my setup and having to work my way Down to the "Optimum" recipe. I believe that taking this route would mitigate the potential detrimental affects of giving underpowered hobby mills the benefit of the doubt and assigning them the power or horse-power rating than the marketing hype would lead us to believe. Tim M.

I agree with you completely about the power ratings that Tormach assigns to it's mills. This is the point I was trying to make with my long winded post. I wish I'd known about editing the specs of my machine before my trial expired. I'll start saving up my spare change. Eventually I'll get a short duration version of your software to try out for a little longer period of time. I'm up to my ears in scheduled work again this week but next week I'll have some free time to try using the latest HSMAdvisor recipe on my last piece of 303 stainless steel round bar. At least I know now that the re-configured charge handle is going to work in its modified shape. That's what I was really hoping for with this project. Using HSMA software was just my attempt at cutting down on the time it took to make it. I'm still learning. Next week I'll find out if HSM is going to work for me. Tim M.

I've run a Tormach 1100 (back in the day, a few years ago) and we used the Tormach Tooling System (TTS) for all of our tools. The system does have sidelock holders, however they are still held by a R8 collet to mate to the spindle. We had some slippage issues similar to what you were mentioning. I did not have HSMA at the time so I can not offer feedback directly regarding the feeds and speeds, however that is also a limiting factor to that particular toolholding system. Pretty sure the issues were typically in 303/304/316(ugh) stainless. If I were still running that machine in and had HSMA I would probably attempt the following: 1. Choose material (303ss) 2. Set up tool, be very accurate with stickout lengths/flute length/diameter which it seems you have done 3. Since you know your DOC and are cutting from the side I enter the DOC I will be cutting to, I let HSMA calculate the optimum WOC. Even if the DOC is HIGHER than the original recommendation. It has to have somewhere to start, and I usually put in the DOC I will be taking. Use more of the flutes of the tool. And the tool is way more rigid cutting near the shank. Sometimes you will have a WOC that you need to hit, and you can let it calculate the DOC. I always let it pick one or the other. 4. I do not use the HSM or Chip Thinning tick boxes. I may some day but for simplicity, and a light machine I think leaving them off is prudent. In fact I think this may be where a lot of the issue is stemming from. Most of the other stuff I think you are doing similar to me. 5. Use the 3 sliders (S, F, Performance) to adjust the cut to keep the HP and torque down to 50-60% or less. You may have to click the chevron to see the performance slider. 6. Profit! Using this formula I came up with following screenshot. Again its been a few years since I've run a Tormach but you will definitely need to keep it dialed back from 100% on everything HSMA says. A few general machining hints: Don't ever cut into a tight corner (I think you know this) unless you are trying to save scrap carbide for retirement. Use a smaller endmill and interpolate. On the Tormach smaller end mills will cut better because it is a light machine anyway. That machine was sold to make space for a 30hp VF-2 that will break the 1/2" bolts holding the vise down before it bogs but those Tormachs are fun little machines, perfect for a garage workshop or small (real small) job shop. I have completely stalled our 7.5hp MiniMill trying to run a M24x3.0 cutting tap into 1018 2" deep. Load meter went to 200% and it just shut down. That was a treat to fix. Didn't even nick the tap though. Good luck. I hope I help rather than hinder (and break any of your tools!) One self taught....machinist-ish to another :ernaehrung004: Jake

My calculation

Thank you for pitching in, Jake. I totally sign under each of your words. But I have to wan, though about going below 50% in feedrate. This may cause excessive rubbing and perhaps work-hardening. Especially in stainless. May be fine in free machining 303, but I would be weary of that. Cheers!

Before actually doing any machining on 303 stainless, I did some informal research on how one would mill this metal. I seem to remember reading that it had the tendency to "Work-Harden" if milled to shallow or with to high of a spindle speed. Unfortunately, I don't know exactly what depth is considered so shallow as to become conducive to creating a "Work-Hardening" situation. I took a look at the screen shot posted by ndisjk. I'm pretty sure my Tormach 770 would bog down to a stop using that particular recipe. The Tormach 1100 is a little more powerful than a 770 so comparing their abilities is not quite an "Apples to Oranges" comparison; it's more like a tangerines to navel-oranges comparison. I guess the same HSM principles apply with either machine. It's just the feeds and speeds that are different by necessity. Tim M.

Tim: As I stated it has been a long while since I ran that particular machine. I was just trying to give you a process to determine your own numbers. With the new machines I run currently I have never run into a work hardening issue in 303. 316 is a different animal, but I do get what you are saying with the lighter machine (just like the story I posted about the big tap in minimill) As far as rubbing: I only use the sharpest of sharp carbide tooling. I have 2 drawers full of 1/2" carbide endmills and have a really really good shop do all of my resharpening. I think this helps a lot with letting the tool cut at low engagements. I often will program 0.0001 or 0.0002 of compensation to really dial in a cut and as long as the tool is sharp it will cut. Perhaps I will record some GoPro video of what I mean. I know I'm actually doing it "wrong" but I've made some incredibly tight tolerance (+-0.0002 13" diam bearing races) by walking them in a couples tenths at a time. Just lends credence to the ole "more than one way to skin a cat" saying. Also: I've had a lot of those "there is no way this will work" moments since purchasing HSMA. It's actually insane what the machines and tools can actually handle. I hope you can get it all figured out Tim, please continue to post your findings as I am rather curious at this point. Jake

Thanks Jake: I spent most of this Sunday running some new numbers using 304 Stainless as my metal stock. Why? Well, I decided to go at this project a little differently than I was doing it with the 303 Stainless Steel. With the 303 Stainless I wasn't able to get any short lengths of flat bar locally and buying it on line was a bit more than I wanted to pay. I was having to buy Round-Bar and trying to mill it down to the dimensions I needed before actually machining it to the shape of my part. What I decided to do was to make a set of "Soft-Jaws" that will hold a short length of 1/4" thick 304 Stainless Flat-Bar. I can get pre-cut lengths of 304 Stainless really cheap locally. This means that although 304 may be a little trickier for me to figure out how to mill. If I screw up I can get more of it without breaking the bank plus; I don't have to remove nearly as much materials to form the shapes I'm after. I think I'm all ready to give it a try now. I installed the HSMA software and I edited the horse power rating of my milling machine. It's just a matter of getting the free time to actually do the milling. I don't want to look to far past this part of this project but, once I get this Charge-Handle whittled out I then have to fabricate the Flip-Out-Lever that will be attached to it. I'll be able to make the Flip-Out-Lever out of softer metal so I'm not to concerned about that part of this same project. I hope I edited the motor specs of my mill correctly. One thing that kind of mitigated some of the stress of relying on the HSMA feeds and speeds recipes is the fact that now that I don't have to removed as much material from my metal stock, I can input much lower DOC and WOC numbers into my calculations. I still have to force myself to trust the numbers that this software has calculated though. Given enough time, I'll begin to figure out what to look for in terms of the calculated recipes. I'll post pics when I finally get them done. Tim M.

I found myself with a little free time in between scheduled income producing work so I thought I'd get started on the "Soft-Jaws" I mentioned in my previous post. I was able to complete them to where I felt they were good enough for this "One-Off" project. In this case, it turned out that "Good Enough" wasn't quite good enough. Fresh out of my Tormach CNC mill the "Soft-Jaws" were straight and true but I did some post machining work on them in my little Harbor-Freight mini mill and that work may have made my straight edges just crooked enough to effect my finished part. Unfortunately, I didn't know this till I'd finished milling my actual part in 304 stainless. On a positive note: You should have seen the finish I was getting with that 304 Stainless Steel. Using my edited motor power within the HSMA software and a slightly tweaked recipe I was getting near mirror finishes and virtually no bogging down of my 1 horse power machine. I did manage to break another end mill; a little 1/8" carbide 4-flute. It had nothing to do with the software or the feeds and speeds and everything to do with me not entering the correct tool offset. I buried that sucker nearly a half-inch deep into my aluminum "Soft-Jaw" stock before it snapped. Something I noticed when I edited the horse power of my Tormach 770 mill in the HSMA software was the fact that even though I reduced it from one-horse down to .75 horse power, the software seemed to want to round it off to .80 horse power. I noticed this same phenomenon sometimes when I entered my numbers in the WOC and DOC text fields. It seems like the software tends to want to round off my numbers to the next highest even number. Also; for my smallest end mill, when I enter WOCs in the .002" thru .009" range, in the "Data" display the WOC reads 0.00". I'm not sure why that is. I guess it could be any number of reasons. Tim M. In the case of my horse power, I still felt that .8 horse power was giving my little hobby mill to much of the benefit of the doubt in terms of power so I went back in and edited again. This time I entered .7 horse power. It was at this level of power rating that I was getting the recipe for the near-mirror finishes I was getting in that 304 Stainless Steel. I've already made up a new set of more precise "Soft-Jaws." Now it's just a matter of finding some more free time. This time I'll be going into this project with a little more confidence in the feeds and speeds recipes I'll be using. I've also ordered some more 1/8" coated end mills for the finer mill paths. Things are looking up. Tim M.

Tim, I am glad you had that figured out. Getting the machine settings figured out is by far the most important part in cases like yours. The number rounding issues you are reporting are just what is displayed to you. They do not really affect anything and stuff is being rounded down in order to improve readability. I am going to tweak that a little to work better for smaller cuts and machines. Regards.

Regarding the numbers being rounded up or down by the software itself, I just thought because (In My Case) my initially entered WOC numbers were so shallow, (using the smaller end mills with a lower powered mill) it was done so, so that the end-user could determine on their own the exact WOC they would eventually go with. I can see how in certain milling operations where harder types of metals are being machined, this could cause that "Skimming" or "Work Hardening" problem I've heard about. Here too, I thought maybe the software was taking that into account and rather than listing those widths of cut of .002-.009 it just listed a default number of 0.00 instead of the shallow numbers I'd entered. At any rate, it's good to know that this rounding up or down of the entered data isn't a glitch of some sort. For the type of machining I do, it doesn't really matter to much any way. I'm just happy that I'm finally beginning to make some sense of it all. There's still alot to learn but at least I'm starting to grasp the concept of HSM. Tim M.

I finally got my 304 Stainless Steel Charge-Handle component machined. I screwed up three out of my four attempts but I eventually managed to get it done. The finish right out of the mill looked outstanding. There is alot of hand-fitting still required as post-milling operations but, this is not the fault of the feeds and speeds calculations; more the fault of the designer of the re-configured Charge-Handle. Once I've hand fitted the parts I can then go back and tweak my CAD drawings to minimize any future post-op work on these same parts. It's like most of my other projects; about the time I get to the end of each project, I've figured out ways I could have done it easier or better and more efficiently. Although this particular project is working out just as I'd dreamed it would, I now see where it can be improved in both form and function. The HSMA software is just helping me arrive at that end sooner. I still have a little more hand fitting to do to get it just right. I'll take some photos then and post them here so you all know what I've been trying to accomplish by using the HSMA software. For the most part, the feeds and speeds recipes that this software has been giving me have fairly reliable. I say, "Fairly Reliable" because the recipes still appear to be a bit to aggressive for my 770 Tormach hobby mill. I find myself having to back off of the recommended WOCs regardless of materials being milled; not so much on aluminum but, mostly the ferrous metals. Just as an example: when I enter a DOC of .250" for a given metal stock and the software calculates what it considers the optimum WOC, whatever that WOC it recommends, I have to reduce it by at least a third in order to keep my Tormach 770 from straining or bogging down as it tries to make those cuts. I don't know about anyone else but there a massive amount of "Pucker-Factor" that takes place every time I can tell my little mill is struggling. It's like having to watch one of your kids getting his ass kicked by a bully who is not as tuff as he thinks he is if you know how to deal with him. That's where learning how to use the HSMA software comes in. Another frustration I've encountered is when I've gone back into the HSMA software and re-entered all of the same data into the pertinent text fields in order to confirm that the previous recipes were what I saved them as. The feeds and speeds data that I used to machine my 304 Stainless Steel Charge-Handle for example; I re-entered the same numbers and the same tool and the same metal stock and the software gave me a recipe with feeds and speeds completely different from what I used to mill that piece of stainless steel. I checked and re-checked to make sure It wasn't just me entering the wrong information but, I can't explain it. It's got me a little confused. From now on I think I'll just use the recipes that the HSMA software initially churns out and work with that. On a positive note; Back when I machined my parts using conventional milling , I could run my fingers along the cutting edge of my end mills and tell that they were no longer as sharp as they were when I first bought them; and this was after just a couple of milling projects. I've machined four different Charge-Handles from three different types of metal using the same end mills and they still feel as razor sharp as the day I bought them. I know this isn't a very scientific way of measuring the sharpness of one's end mills but, that's just how I do it. With the HSMA software I can now use all the cutting edges of my end mill instead of just the tip. Tim M. MetalShavings

Tim, I am glad you are making such great progress. Regarding the reported saved speeds and feeds not matching between then and now. This is because you (as I suggested) reduced the available HP of your machine. With less HP it will suggest lighter cuts. Which in turn will change the kind of numbers you see. This behavior is totally normal due to the fact that it is not possible for the Calc to display the old numbers and still fit them under the new HP restrictions. Let me know if you have any other questions. Regards.

I finally got a chance to take a couple of pics of my K31's reconfigured "Charge-Handle." The photos were hastily taken so they're not the best but, I'm hoping that they give you an idea of what I've been trying to machine using the HSMA software on both 304 Stainless Steel and 1018 steel. Since arriving at this point in this project I've come up with a slightly more refined configuration of this same project. This means that the parts in these photos are now relegated to just another set of working prototypes. I think the next finished group of "Charge-Handle" components will be the final working parts I'm looking for. Because of the power limitations of my Tormach 770 hobby mill the time it took to do the actual machining using the HSMAdvisor software was somewhat faster than it would have been had I used the conventional milling techniques I was accustomed to using. I was wondering; Since the Tormach 770 hobby mill is driven by pulleys and a belt that allows for two different pulley positions, would changing the position of my drive belt to the Lower-RPM position offer any benefit in the form of higher torque over the Higher-RPM pulley setting when running the HSMA feeds and speeds? I'll have to look it up to confirm but I think that when set to the Lower-RPM pulley my the torque may be increased; which might mitigate some of the bogging down that I've encountered when I run my mill on the 10,000 RPM pulley. I'll have to check but, I think that when my drive belt is set in the Lower-RPM pulley the maximum spindle speed is about 5,000 RPM.

comparison of factory and project Charge-Handles What it looks like when assembled

Tim, changing to lower RPM pulley definately will increase your torque and help prevent stalling. Regards.

Hi Tim, I uploaded a Low range Tormach 770 machine to the cloud for you. According to the data i am getting you would not see any benefit using the low-range pulley when doing HSM Machining. Tormach has a dip in power curve towards the max RPM and i am afraid you will not even get more torque there. Please try it if you can and let me know how it goes. Perhaps i ought to revise the Tormach power curve model. Regards.

Hey Elder: You would think that for a guy like me who walks around with his head in the clouds all the time I'd know what you were referring to but, What cloud are you referring to and how do I get there? I don't have to smoke anything to access whatever you're referring to do I?http://zero-divide.net/smiles/blink.gif I quit doing that stuff a long time ago. Is there some kind of internet link that will get me there? Thanks TIm M.