Help with Parameters
Login to Your Account
Likes Likes:  0
Results 1 to 2 of 2
  1. #1
    Join Date
    Jun 2021
    Post Thanks / Like
    Likes (Given)
    Likes (Received)

    Default Help with Parameters

    Is there a general rule anyone has for getting the best surface finish on mild steel such as 1018, 1045, 1215 etc..? I am working with a 4.5" x 11" .750 thick piece of Flat Hot Roll on a Haas TM-2, using a 3/4 carbide endmill. My DOC is at .5 with a WOC at about .015 as for my speeds and feeds I am at 2,000 rpm and 60 IPM. It cutting fine however I am just a "Young Buck" as others in the trade would call it and was wondering if there were any tips for achieving the following

    1. The best surface finish on the last pass.

    2. Best Parameters for a nice, quiet, efficient toolpath

    3. Tips and rules of thumb as far as applying it to other size cutters.

  2. #2
    Join Date
    Jul 2020
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    In my experience, finding the right feeds and speeds really comes with trial and error. A 3/4" endmill is pretty broad in terms of what brand and style that refers to. Even when you have near identical tools from 2 different manufacturers, you can get wildly different results. The holder and work holding also play a factor in how the finish comes out.

    A typical approach would be to take it slow and try to get the surface finish you desire. Once you're have it looking good, increase the feed and speed together(to maintain the chipload which is the primary driver for finish quality) until the harmonics start to take over reducing finish quality. You can break through ranges of harmonics usually increasing the chipload(dropping speed or increasing feed) until you find the sweet spot that your specific setup/machine like.

    Your machine, will play a bigger role than you might think here as a TM-2 isn't by any means a heavy duty or even medium duty machine. And machine rigidity is quite important when you start to reach the limits of your cutter's performance and even your tool holder's capability for making a solid connection between the tool and the spindle itself(usually more apparent when roughing).

    So, let's say you have a general purpose 4 flute endmill and you squeeze all the feed and speed out of it you can. I'd say the next step would be to find finish specific type 5-7 flute endmill for steel. By increasing the number of flutes you lower the chip per tooth when using the same feed/speeds as your 4 flute. So, increase the feed to compensate. And being that 5-7 flute endmill's have a larger 'core' between the flutes, the cutter will be more rigid as well allowing for better resistance to vibrations and deflections.

    From here you can experiment with variable index flutes(asymmetrical flute orientation around the tools axis) as well as variable helix flutes(gradually increasing helix angle along the flute length) to get even more performance. And then from there it really depends on what the machine can handle.

    In a TM-2 you don't have a ton of power and rigidity, but you may have enough speed for a trochoidal adaptive roughing routine. You also don't have much space for extra tools so you may need to rough and finish with the same tool. So, for this situation I would probably find a rather standard 5 flute, variable helix, AlTiN coated cutter and see what I can get out of it. If I'm doing hundreds of the same part, I may look to a something that cost's a bit more but gives me longer life, better finish, and gives me a better ROI overall.

    Really try to find a good set of generic tools that you know and like and try to find their sweet spot. Then, as you get more jobs that allow you to maybe spend a couple hundred extra on a new style of cutter, then you can start to see what works best for you, your machine/setup, and your wallet.

    Sorry, I can't give you a more detailed answer about feeds and speeds. What you have listed seems to be nice starting point to work from. All one can really do is experiment. The best rule of thumb here is just starting at conservative SFM. For me, that can range from 100 to 250 SFM for finishing steels. And well beyond that when roughing with a trochoidal path. The longer the flute and stickout from the holder, the lower my starting SFM will be.

    Another thing you might want to consider is your chip thinning calculation. With a 4fl .750" @ 2000rpm(392 SFM) and 60IPM, your chipload at full radial engagement is .0075", but your actual chip thickness is .0011" because your stepover is only .015". Some might say you should take .005" stepover for your final pass or maybe even .001". But in some circumstances .015" maybe the magic number as the cutter/holder/setup combo doesn't generate harmonics due to the increased cutter pressure. This can cause more deflection which may require you to do an additional spring pass anyways, but increasing to a 5 or even 7 flute can help alleviate the tool's deflection and susceptibility to the harmonics and not require that additional spring pass.

    Anyways, good luck and experiment as you can.


Tags for this Thread


Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts