#### By MetalShavings

#### 41v50 Rifle Barrel Steel

It's been a while since I visited here. I've been setting up to do some Spiral Fluting on an incoming rifle barrel project on my Tormach 770 mill.

Setting up everything including the 4th-axis is pretty straight forward. Working on typical 4140 and stainless rifle barrels isn't really hare either but, my apprehension here has more to do with metal alloy I'll be working with in this barrel project.

I've run the numbers in my copy of HSM Advisor and I'm coming up with some feeds and speeds numbers that kind of leave me scratching my head.

I'll be using a 30 degree helical 4-flute coated carbide end mill. My flute length and stick out is one inch. It's a typical configuration ball nose end mill. My DOC is only .008" and I'm running it with the "Pocketing" box checked. The alloy that this barrel is made of is 41v50 steel. I had never heard of this type of metal till I came across it when purchasing this sample barrel. Apparently the military uses this alloy on their AR platform rifles for durability and rigidity.

My reason for posting was to ask; has anyone here ever worked with this metal alloy? Also. I've deliberately not listed the feeds and speeds I came up with because I wanted to ask those of you who may be willing to run the numbers in your version of HSM Advisor and see what you come up with. It may be that there's something I'm missing or inputting incorrectly when I enter this info in the their respective text fields.

I can tell you that any time I do any milling with my One-Horse-Power Tormach mill I have to back off of the actual speeds and feeds I'm given by at least two-thirds. With hard metals like this 41v50 I'm thinking that I will most likely have to back off even further than two-thirds.

I'll check back here later in hopes of someone being kind enough to run these numbers to see how the numbers they come up with compare to what I've came up with. Thanks in advance. If more information is needed please let me know and I'll make sure to include that with a reply.

MetalShavings

## Eldar Gerfanov

Hi,

You did not specify what diameter the tool is, so i assume its 0.5"

If you only do one pass slotting at 0.008" deep, then check the first screenshot.

I use 2 flutes because a 4 flute ballnose end mill has only 2 flutes cutting at that depth.

If you are actually making multiple 0.008 slotting passes to get to (for example) .125" depth, then you need to calculate as if you are slotting at 0.125". In this case you should set the number of flutes to 4. See the second screenshot.

You should provide more info because a seemingly insignificant detail may cause significant change in parameters for ball nose cutters.

A ballnose end mill may exert large cutting force on your machine, so do not forget to adjust for your machine rigidity.

Best regards.

## MetalShavings

Hi Eldar:

I knew this was going to happen. I mean forgetting to enter more pertinent information. Actually I planned on using a 1/4" diameter 4 flute coated carbide ball nose end mill. It will be done in multiple passes of .008" each and the full depth is only .048" deep.

Why am I doing these spiral flutes this shallow? It's because I only want to score the surface with the spiral pattern I've modeled. I don't want anything deeper than this. Initially I was going to make the flutes .10" deep but when I calculated the numbers my feed rate was so slow that it was more a kin to a crawl-rate rather than a feed rate.

My HSM Advisor software was telling me that I needed an RPM of 10,000 and a feed rate of 3.7. With was with me backing down the feed rate to accommodate the low power of the mill and to minimize the torque and deflection of that skinny quarter inch diameter end mill.

I am glad to see in your screen shots that you picked as the metal alloy the 4150 alloy that was the harder of the two 4150 alloys that are listed in the drop down menu. At least I got that right.

Would you suggest using a two flute coated carbide end mill instead of a 4 flute? This project is still in the working stage so if something like a 3/8" end mill might be a better fit for this kind of spiral flute project (especially on this type of hard alloy) I still have a bit of time to order one to use instead of the 1/4" ball nose I initially intended to use.

Thanks for the quick reply.

MetalShavings

## MetalShavings

I also needed to mention that in your screen shots you have listed as your milling machine a 30 horse power VS series Haas. Mine is a one horse power Tormach hobby mill and when I entered my numbers to get my calculation I too checked on the "Slotting/Pocketing" check box to activate it.

I didn't notice that difference in CNC milling machines when I first viewed your scree shots. I really loved the numbers you came up with when I first saw them. Even if I had to reduce those number by two thirds they still would have been faster than my numbers. That's when I noticed the difference in hose power and rigidity.

I really just want to confirm that the snails-pace numbers I came up with are somewhere close to being right. If I have to run a real slow feed rate I'm OK with it. I just want to make sure my feeds and speeds are good for the task at hand.

MetalShavings

## Eldar Gerfanov

Hi,

Machine type actually does not affect anything in this calculation.

The HP requirements are so low, that it does not matter Tormach of HAAS.

There is stiffness issue of course, but it should not make too much difference.

Couple of points to make your machining more successful:

1. Most important: Use stub length end mill.

If you need reach, then you can stick it out further, but try to get the shortest flute possible.

1" long flutes that you mention is very long. your endmill will flex all over the place

2. Use 2 flute coated carbide endmill.

3. Use coolant: it will help you with heat buildup and friction in the tip.

I personally would start with the parameters as per screenshot.

But yet again i have not worked on Tormach, so you might want to start 50% slower in both the speed and feed.

Good luck!

## MetalShavings

Many thanks Eldar:

I notice in this latest screen shot this time around you do not have the "Slotting/Pocketing" box checked off. Is there a reason for this other than possibly forgetting to check off that box? It could be that it's not really needed in this type of milling operation, I don't really know. That's why I'm asking.

I'm happy to see the numbers you've come up with but it still leaves me scratching my head. With the exception of the "Stick-Out" and "Flute-Length" differences (and not checking off of the "Pocketing" icon) I entered basically the same numbers as you did and got some very different numbers. No matter; I would much rather work with the numbers you got than the numbers I initially had gotten.

My barrel blank should arrive next Tuesday so that will give me some more time to order a shorter quarter inch cutting tool for the job. I plan on doing some test cuts on some Delrin rod stock just to make sure my tool paths or OK. I still have to thread and chamber the barrel before I get to the fluting stage of this project.

I'll let you know how it turns out. Thanks again for your help. I really appreciate it.

MetalShavings

Tim M.

## Eldar Gerfanov

Hi Tim,

The Even though "Slotting" is off, WOC is the same, so it does not affect anything.

I am not sure why you are getting very different values.

Please send me a screen shot of your HSMAdvisor window with all panels expanded.

Regards.

## MetalShavings

I'll try to get that screenshot tonight if I can figure out how to do it.

MetalShavings

## MetalShavings

For the last couple of nights I've been trying to get that screenshot I promised in my last reply. No matter what information I've entered in the text fields I can't get it to churn out the same results I got the first time I tried.

The first time around I entered all the data I listed in my initial post on this thread. Entering that same information I'm now getting numbers that more closely resemble the numbers you came up with when you were kind enough to run similar numbers in your version of the software. I did find one difference in the data we input. My Stick-Out was listed at one inch with a flute length of one inch as well. Yours is listed as .625" and .500" respectively.

I'm not sure if that could account for the major difference. In my initial calculations I also lowered my feed rate to minimize the torque and deflection so maybe it was these three settings that gave me those initial feeds and speeds of 10000RPM and 3.7in/min.

I'll keep looking for the source of my error as time permits. I'll also remember to post the results once I get this project done.

Thanks for your help.

Tim M.