[MetalShavings]

I recently came up with a fix for one of the trigger components in my air rifle that now gives me what I would consider to be a "Match-Grade-Trigger" pull. I sent out several samples for testing and with input from the testers and further tweaking I've been able to come up with a finished product that will fix the trigger pull nightmares of anyone owning and shooting this particular brand of budget air rifle.

I've already machined several of these little steel replacement trigger parts but now, I've had several guys ask me to make them a replacement part for their air rifles.

When making the previous batch of steel components I used the "Wizards" in the Mach-III software to calculate my speeds and feeds but, one of the things that continues to baffle me is the correct depth of cut for any given metal, cutting tool, surface finish or tool path.

I'm making these tiny little parts out of 1018 metal stock. On my Tormach 770 machine, I'm using both a square ended 1/4" 4-flute and 3/8" 4 flute coated carbide end mill that stick out of the tool holder about an inch and an eight. I seem to be able to come up with the appropriate feeds and speeds OK, but I'd like to know what the optimum depth of cut for each of these cutting tools would be in order to mitigate tool wear and maximize production time.

Other than the rudimentary "Wizards" software, I don't have any other means of calculating depth of cut so I was hoping that one of you guys with the G-Wizard software could clue me in to the appropriate depth of cut for these parameters. Also; is there a general rule-of-thumb regarding depth of cut for those who don't have the software or the math skills to calculate? I absolutely SUCK at math so I find myself taking very shallow depths of cut out of paranoia; and to shallow of a cut can be just as detrimental as having to deep of a cut.

So I'm asking for help from some of you more experienced chip makers. Thanks in advance.

MetalShavings

[Philbobb]

FSWizard - Free Advanced CNC Speed and Feed Calculator


Depth of cut will be based on what your mill and end mill will handle based on horsepower and rigidity. Plug in numbers up above, and keep an eye on the tool deflection and horsepower for the cut. If you slot you're generally going to be shallower on DOC, deeper is better for tool useage but you'll need a narrower width of cut. Take 30 minutes of your day to do test cuts in materials you'll use with the end mills you'll use.

[MetalShavings]

I checked out the link you listed and it appears that the numbers I come up with using the "Eye-Balling-Method" of determining depths of cut when using the "Wizards" in the Mach 3 software are not to far off from the numbers I'm getting with this online calculator. In fact, the feeds and speeds numbers are extremely close to what I'm already getting. Being mathematically challenged, all of those numbers are just mind-numbing to me. And I'm not really clear what I'm looking for in terms of tool deflection or the "HorsePower" or "Torque". I did note that they seemed to display in red letters. I don't know if this is because something is wrong or if this is how they typically display.

Am I shooting for "Zero-Tool-Deflection"? And what about "Horse-Power"? What is that all about? I can get zero tool deflection if I leave my tool on the tool rack but I won't get any work done; Ditto with the horsepower. There must be an optimum number that I'm looking for with respect to these two items but, right now I don't have a clue what that is.

With respect to the DOC, I must be mistaken in my assumption that entering all of the pertinent numbers or work parameters would automatically get this software to calculate an optimum depth of cut. I guess it doesn't work that way. Or maybe I'm going about it wrong.

At any rate, many thanks for your response. I think it will get me moving in the right direction. I'll keep looking for answers that my brain can process.

MetalShavings

[SCzEngrgGroup]

You have to configure the tool for your machine - there should be a preset for both Tormachs. Once that's done, RED indicates a parameter that is not safe, and you will either stall the spindle (HP or Torque red), don't have enough RPM (RPM red), or will break the tool (other parameters red).

Regards,
Ray L.

[Philbobb]

You have to configure the tool for your machine - there should be a preset for both Tormachs. Once that's done, RED indicates a parameter that is not safe, and you will either stall the spindle (HP or Torque red), don't have enough RPM (RPM red), or will break the tool (other parameters red).

Regards,
Ray L.

The free online version has no presets for machines. For some weird reason it always shows the torque and deflection in red, maybe to highlight them?


Keep the horsepower below your mills peak, so below 1hp. I find that my 1100(1.5hp) sounds like it's straining when FSWizard shows a cut of 0.9-1.0hp or greater at 5100rpm. I can go a little higher on the estimated hp if I stay in the 4000rpm range. Your 770 is going to be different, that's where experimenting comes in.

When trying out cuts I will start out with a shallow DOC, say 0.05" and see how it sounds. Depending how it sounds I will increase DOC from there by 0.05 or with steel 0.025" and try again. I try to be on the safe side and always go with numbers for slots/pockets, unless I know my WOC won't ever be over 50% tool engagement. Plug in the numbers for what you do right now. Note the horsepower that FSWizard spits out, then proceed from there. Your 770 is going to be limited on horsepower at the rpm you would run a 3/8 end mill at in steel, keep that in mind. If you run into chatter, spindle struggling, etc decrease DOC and/or WOC. Don't decrease feed rate without decreasing rpm or you may make it worse or cause rubbing - tool rubs the steel but doesn't cut it.

[SCzEngrgGroup]

The free online version has no presets for machines. For some weird reason it always shows the torque and deflection in red, maybe to highlight them?

Interesting. I think he's probably just trying to highlight the important numbers. On HSMAdvisor, once you setup a machine profile, it will keep within the machines limits, and highlight in red any values that you've forced to excessive values by going too deep, too wide, etc.

Basically, I would look at HP (keep to no more than ~1.0 for the 1100), tool deflection (keep to a few tenths for small tools, and under 0.0007 or so for larger ones, like 1/2". Do test cuts, starting at about 60-70% of the recommended feed, and see how it cuts. If it's ok, then try 80%, then 90, then 100. Every machine, and every tool is slightly different, so don't expect feeds and speeds optimized for one brand of tool to work well on another. Find ones that work well for you, and stick to those.

I use HSMAdvisor, and it never steers me wrong. It's about the best money you can spend if you want to protect your tools, and increase productivity. The mobile version is handy to have on your phone or tablet.

Regards,
Ray L.

[RussMachine]

By experimenting, I've found out that roughing end mills use ALOT less horsepower than traditional 'smooth flute' end mills.
I always hog out my parts with a roughing endmill, then finish with regular end mills.
I cut 1018 steel at full depth, (.687" deep), at 1500 RPM, but only remove .100 on the side cut, using a 1/2" rougher.
No problem with stalling.

[MetalShavings]

I down loaded the trial version of the HSM software and gave it a try. It does list the tormach 770 and its parameters. It appears to calculate as expected. My problem was that I was expecting this or any software to calculate the correct or optimum DOC based on the feeds, speeds, metal stock, horse power, etc.. This does not appear to be the case. In fact, it appears to be nearly the opposite of that. It uses your chosen depth of cut to calculate everything else and warns you if something is wrong.

Strangely enough, the calculated numbers that this HSM software is churning out aren't all that different from what I'm getting from the rudimentary Mach 3 Wizard's calculated numbers. Even with my unscientific "Eye-Balling" method of calculating the depth of cut, it's starting to look like the DOC's I was choosing were within the safe parameters of my 770's and my tooling's abilities.

Still, in the back of my mind is always that lingering feeling that the numbers being calculated by these softwares may not always be the best. I guess it just takes more hands on experience rather than text book reading. It's easier for me to understand the chatter of a cutting tool and the straining of a motor than it is to read the written word that attempts to describe it. There's gotta be an easier way.

The depths of cut that came up by just entering the cutting tool description just seemed outrageously deep. I could just picture my end mill breaking as soon as they made contact with my metal stock but, who knows. It could just be a case where I haven't come to fully rely on any software to determine how I break my tools.

MetalShavings

[SCzEngrgGroup]

I think you're looking at it backwards. You don't decide the RPM and feed you want to use, then see what depth/width you can use. You look at the material you want to remove, and decide what the best depth/width are, then calculate RPM and feed. Where HSMAdvisor really shines is if you're able to HSM machining, and take advantage of chip thinning, and other factors, to drastically increase your throughput. As an example, my typical roughing cut in 6061 uses a 1/2" HSS 2-flute, running at 5900 RPM, 110 IPM. the "old school" way would have me running under 3000RPM, and under 30 IPM. At the higher speeds, I get higher MRR, less stress on the machine, better finish, and longer tool life. But, you have to have appropriate toolpaths, or you'll just break tools left and right.

For the record, HSMAdvisor calculates based on many equations, and the authors extensive experience as a machinist. NOBODY gets optimal results without factoring in experience, and no tool will give you optimal values for YOUR tools, and YOUR machine. That comes only from letting the tool get you close, then doing test cuts to see where the limits are for your particular machine, tools, and setups. You'll never get optimal results until you have enough experience to know how to "read" the sound and feel of the machine, and the cutting results. No software can replace that knowledge.

Regards,
Ray L.

[mountaindew]

I would like to add something to consider. Most the advice above and in fact most of what I read anywhere is focused on feeds, speeds and material removal rate. Being a newer user I find fixturing and how well I can hold onto my material a major factor also. Larger tools that can work with high feed rates, doc and woc tend to be fine when you have big parts that you can hold onto. I tend to do small parts and this gets me thinking more about if the material is going to move in the fixture then anything. From your description it sounds like your also doing some small parts and might need to consider this. In the end I find myself with 1/8 end mills chipping away at little features on my parts and high feed rates and doc/woc are not possible without tool deflection or damage and the majority of the time to make many of my parts still ends up in these operations.

[MetalShavings]

I think you're looking at it backwards. You don't decide the RPM and feed you want to use, then see what depth/width you can use. You look at the material you want to remove, and decide what the best depth/width are, then calculate RPM and feed. Where HSMAdvisor really shines is if you're able to HSM machining, and take advantage of chip thinning, and other factors, to drastically increase your throughput. As an example, my typical roughing cut in 6061 uses a 1/2" HSS 2-flute, running at 5900 RPM, 110 IPM. the "old school" way would have me running under 3000RPM, and under 30 IPM. At the higher speeds, I get higher MRR, less stress on the machine, better finish, and longer tool life. But, you have to have appropriate toolpaths, or you'll just break tools left and right.

For the record, HSMAdvisor calculates based on many equations, and the authors extensive experience as a machinist. NOBODY gets optimal results without factoring in experience, and no tool will give you optimal values for YOUR tools, and YOUR machine. That comes only from letting the tool get you close, then doing test cuts to see where the limits are for your particular machine, tools, and setups. You'll never get optimal results until you have enough experience to know how to "read" the sound and feel of the machine, and the cutting results. No software can replace that knowledge.

Regards,
Ray L.

Huh: I thought that this was what I said in my previous post. Oh well.

The way I've been doing it was to let the Mach3 Wizard calculate my feeds and speeds by entering tool dimensions, metal type an such. That is how I get my feeds and speeds. Then, using my naked eye, I'll figure the depth of cut by what I feel will work for the speeds and feeds the have been calculated.

As I stated before, it's not very scientific but, it appears to be working for me. My reason for initially posting my request for help with the finding of the optimum DOC was because I thought there was some way or some software that would do it for me. It looks as though I was mistaken.

I'll just keep doing it the way I was doing it and hope for the best as I'm traversing that learning curve.

My thanks to everyone who took the time to give their input. And by the way; I agree with what mountaindew has stated but, the work-holding in my case is about the only part of this parts run that seems secure.

MetalShavings

[SCzEngrgGroup]

Workholding is absolutely VERY important, but even on small parts, you can use HSM if you fixture properly. Here is the first of 12 parts I made for my toolchanger a few days ago, done mostly using a 1/2" EM at 110 IPM:

Attachment 282502

Attachment 282504

It starts out life as a 0.875 x 1.625 x 1.375 block of 6061. It's gripped by 1/8" on the bottom in a vise, and the 1/2" dia. "shank" is milled at the above feeds/speeds, then it's drilled, reamed, and a O-ring groove is cut in the "shank". It's then turned over, and put into the fixture in the photo, which is just six TTS ER20 chucks mounted to a fixture. It's held by less than 1/2" of that 1/2" "shank", but that's more than enough. The other features are then machined using the same tool, feeds, and speeds. Total machining time is barely 3 minutes per part. There's more time in toolchanges (even with an ATC) than actual machining time.

Regards,
Ray L.

[zero_divide]

I down loaded the trial version of the HSM software and gave it a try. It does list the tormach 770 and its parameters. It appears to calculate as expected. My problem was that I was expecting this or any software to calculate the correct or optimum DOC based on the feeds, speeds, metal stock, horse power, etc.. This does not appear to be the case. In fact, it appears to be nearly the opposite of that. It uses your chosen depth of cut to calculate everything else and warns you if something is wrong.

Strangely enough, the calculated numbers that this HSM software is churning out aren't all that different from what I'm getting from the rudimentary Mach 3 Wizard's calculated numbers. Even with my unscientific "Eye-Balling" method of calculating the depth of cut, it's starting to look like the DOC's I was choosing were within the safe parameters of my 770's and my tooling's abilities.

Still, in the back of my mind is always that lingering feeling that the numbers being calculated by these softwares may not always be the best. I guess it just takes more hands on experience rather than text book reading. It's easier for me to understand the chatter of a cutting tool and the straining of a motor than it is to read the written word that attempts to describe it. There's gotta be an easier way.

The depths of cut that came up by just entering the cutting tool description just seemed outrageously deep. I could just picture my end mill breaking as soon as they made contact with my metal stock but, who knows. It could just be a case where I haven't come to fully rely on any software to determine how I break my tools.

MetalShavings

Hi, HSMAdvisor calculates suggested depth of cut based on your tool type, material and tool geometry. It then calculates ideal speed and feed for such a set up.
It is no wander that numbers may match other calculators output.

But what HSMAsvisor does, it then looks at your machine power, deflection and torque safety limits and limits your feedrate if somethimg is wrong.
It will at the same time suggest you ways of improving your results by usually decresing your depth of cut.

The easyest way to do it is to decrease Productivity slider (expand Speed/Feed Overrides panel to see it). After you do that, it will suggest lower cutting deopth, that will not overstrain your machine.

[vmax549]

It would be easy to Modify the WIZARD to output the DOC based on Feed/speeds AND the available Machine HP.

Just a thought, (;-) TP

[mountaindew]

Workholding is absolutely VERY important, but even on small parts, you can use HSM if you fixture properly. Here is the first of 12 parts I made for my toolchanger a few days ago, done mostly using a 1/2" EM at 110 IPM:

Attachment 282502

Attachment 282504

It starts out life as a 0.875 x 1.625 x 1.375 block of 6061. It's gripped by 1/8" on the bottom in a vise, and the 1/2" dia. "shank" is milled at the above feeds/speeds, then it's drilled, reamed, and a O-ring groove is cut in the "shank". It's then turned over, and put into the fixture in the photo, which is just six TTS ER20 chucks mounted to a fixture. It's held by less than 1/2" of that 1/2" "shank", but that's more than enough. The other features are then machined using the same tool, feeds, and speeds. Total machining time is barely 3 minutes per part. There's more time in toolchanges (even with an ATC) than actual machining time.

Regards,
Ray L.

Some good looking parts! I like your vise stop, simple and useful. Going to draw and cam one up tonight!
Also very neat fixture with the er collet holders. Always amazed by the different ways everyone comes up with to hold on to material.

[MetalShavings]

It would be easy to Modify the WIZARD to output the DOC based on Feed/speeds AND the available Machine HP.

Just a thought, (;-) TP

TP:

Are you one of the programers that configures the HSM calculators? If so, the change you've eluded to alone would be enough for me to actually buy this software rather than having to be downloading 30 day trials or asking for help with this kind of stuff.

When you're a mathematically-challenged dyslexic-hobby-machinist like me, trying to decipher this kind of stuff is like trying to read Egyptian hieroglyphs. I can't make heads or tails of those either.

Most of the machining experience I possess has been arrived at by self-taught means. Taking this route of learning basically means that you have a teacher that is just as ignorant as the student because they're one and the same. It becomes a trial and error learning process.

Don't get me wrong, I'm not completely ignorant on the subject of machining with a mill or a lathe. (I have both) I've managed to learn how to use both with a fair amount of success. I've designed and produced some pretty cool and usable stuff over the years. It's just that the more I learn, the more I know there is to learn.

I finished up the parts I eluded to in my initial post. I used my "Eye-Balling" method of calculating my DOC and it seemed to work just fine for that small run of parts. I can't help but think that there has to be a more efficient way of going about it. Having a calculator that could figure out the optimum DOC for a given parts run scenario would make my machining hobby a whole lot easier. It might even put me in a position where my metal working toys could make me some more spare change.

Once the DOC thing is figured out, then I'll have to move on with learning about how or when exactly to use or not use coolant. The learning is as endless as finding the correct answers.

MetalShavings