Welcome to the Podiatry Arena forums

You are currently viewing our podiatry forum as a guest which gives you limited access to view all podiatry discussions and access our other features. By joining our free global community of Podiatrists and other interested foot health care professionals you will have access to post podiatry topics (answer and ask questions), communicate privately with other members, upload content, view attachments, receive a weekly email update of new discussions, access other special features. Registered users do not get displayed the advertisements in posted messages. Registration is fast, simple and absolutely free so please, join our global Podiatry community today!

  1. Everything that you are ever going to want to know about running shoes: Running Shoes Boot Camp Online, for taking it to the next level? See here for more.
    Dismiss Notice
  2. Have you considered the Critical Thinking and Skeptical Boot Camp, for taking it to the next level? See here for more.
    Dismiss Notice
  3. Have you considered the Clinical Biomechanics Boot Camp Online, for taking it to the next level? See here for more.
    Dismiss Notice
Dismiss Notice
Have you considered the Clinical Biomechanics Boot Camp Online, for taking it to the next level? See here for more.
Dismiss Notice
Have you liked us on Facebook to get our updates? Please do. Click here for our Facebook page.
Dismiss Notice
Do you get the weekly newsletter that Podiatry Arena sends out to update everybody? If not, click here to organise this.

Endmills for polypropylene and EVA

Discussion in 'Biomechanics, Sports and Foot orthoses' started by JTValls, Sep 3, 2017.

  1. JTValls

    JTValls Active Member


    Members do not see these Ads. Sign Up.
    Dear friends,

    I need advice of which endmills you use in CAD CAM to mill orthoses. Recently I have purchased a CNC with a KRESS spindle. I want to change it with a more powerful motor (i.e. Teknomotor 2KW) but first I want to experiment with endmills and materials. I'm newbie in the CNC world.

    WHat endmills do you use for polypropilene? Do you use the same for rough cut and finishing the orthotic device? For EVA i see you use a blurr or ballnose endmills but, for this blurr endmills what characteristics they have?

    If you can, anybody can advice me of what feedrate and RPM you usually use with this endmills?

    Thanks a lot for the help.
     
  2. mr t

    mr t Member

    Hi JTValls,

    The answer to this question is not simple. I will try and answer it in a way that will help others also. Getting the right cutter speed for your CNC router is not always a simple variable and can involve trial and error. I have attached a link to a good website that does have charts for different materials.

    www.cncrouterbits.com.au/technical_speeds_feeds

    When choosing a CNC router, table size does matter. The first question to consider is the space to put it in. The smaller tables are usually chosen because of the available room size, however the smaller the table - the smaller the spindle motor to cut and steppers to drive the axes. This can be compensated for by taking smaller cuts of materials with each pass, thus increasing the time to machine, but adding safety and making it easier on the spindle and steppers. The most cost-effective size to buy is a 1200 x 1200 sized router with a 3.5kW spindle motor. This will give you the least amount of problems for EVA, MDF and polypropylene. If you do not have the room for this the next general size table is a 600 x 900 size table. They usually cost nearly the same amount as the larger sized 1200 x 1200 table. As a note, a 1200 x 1200 table can cut around 12 full length pairs of EVA orthoses at a minimum per run when using an array of pre-cut EVA blanks, while a 600 x 900 table can do about 4 pairs. Routers smaller in size than 600 x 900 generally do not have the stepper motors capable to run a 3.5kW spindle motor. Generally, 2.2kW motors are on 600 x 900 sized tables.

    Conclusions:


    1) 600x900 CNC routers can get 3.5kW motors installed
    2) 600x900 CNC routers cost nearly the same as 1200x 1200 CNC routers
    3) Make sure you can get the CNC router through all the doorways and access points. Generally, a 600 x 900 table on a stand will not go through a standard door. The total size needed is about 1000mm (W) x 1200mm (L). If you need to go through a Standard door you might need to look for a table on a detachable stand.

    The general rule when machining is setting the feed rate to run at a level that does not overload the spindle motor or the stepper motors. If it is overloading you will hear the spindle motor labour, slow down or stall. This can cause the stepper motors to stall and loose steps which will ruin the job. I have found when milling that a 2.2kW spindle motors when attempting to machine high-density EVA in a single depth pass. We recommend a 3.5kW spindle motor for this reason.

    Solutions when using lower powered spindle motor


    1) Decrease the feed rate while balancing RPM accordingly
    2) Decrease stepover to reduce cutting load
    3) Increase number of passes to reduce cutting load
    4) You can also increase the power to the steppers. A rule of thumb is if the steppers are getting too hot you have too much power to them, which will cause damage. If they aren’t being sent enough power then you will stall all the time and loose steps. There is a balance here – and also you need to consider the capability of the motors.

    Spindle motor speed is dependent on the material that is being cut as well as the hardness of the cutting tool. For example, carbide cutters can run at a higher RPM than a soft steel cutter. If you are cutting EVA then an RPM of 12,000 is appropriate at a feedrate of about 1,800mm/min, or higher if the machine can handle it and the material is well attached. If the RPM is too high and the Feed Rate is too low then the EVA will melt into the cutter and make it not cut as effectively.

    We have made a special 15.0mm diameter ball nosed burr cutter with a 10.0mm hardened steel shank for EVA machining. They last for years provided you don't run them into the milling table, or mess up your feeds and speeds. It took years to get that cutter right as they needed harden steel shanks and the process of growing the teeth on the cutter anneals the metal making it soft. Eventually we came up with a split cutter. I have seen nice cuts from multi-fluted cutters, but have found that they go blunt very quickly with EVA as it is very abrasive. When they are blunt the finish tends to be quite rough as the cutters tend to tear more than cut.

    EVA Router Bit: http://podcam.supplies/index.php?route=product/product&product_id=501

    (Apologies for the blatant advertising Craig I can remove if you like)
    When cutting MDF you should consider the number of flutes on the cutter and power of the spindle and stepper motors. A general rule is that as RPM increases so does the Feed Rate. So, if the RPM is set to 18,000 (which works well for MDF) then the Feed Rate for a 2-flute cutter would be about 3,600mm/min.

    The following equations can help you make sense of speeds and feeds for different cutters:

    Chip Load = Feed rate / RPM x number of cutting edges
    Feed Rate = RPM x number of cutting edges x chip load
    Speed (RPM) = Feed Rate / Number of cutting edges x chip load

    We run 2-fluted ball nose carbide cutters for MDF and spin at 18,000RPM.

    You can follow the same rules for poly and you will work it out pretty quickly. You are looking for chips to come off that don't melt together. Too slow and the head loads up and this will cause missed steps and the cutter speed slowing to much or stalling, which can bend the cutter shaft or break it.

    Hope this helps. There are probably people on here with more experience machining polypropylene that can help you out.
     
  3. JTValls

    JTValls Active Member

    Dear Mr. T:

    Sorry for delay. Wow thanks for this answer, i will study you post. In polipropylene i know it can be used normal ball nose, but how many flutes? What direction the flutes need to have?? i think this material at high speeds melt?

    Thanks
     
  4. Phil Wells

    Phil Wells Active Member

    Hi JT

    A good of thumb for PP endmills is to mimic the tool geometry for the cutting of aluminum. I prefer a 45 degree draft on a 2 or 3 fluted device. I also prefer high speed steel (HSS) as this has slightly more flex than carbide, is cheaper and can be re-sharpened quite a few times - big money saving.
    However Anthony's comments about tweaking things for the specific machine are really important as even between models by the same manufacturer of machine you do get differences. Some very clever person at Delcam created a piece of software for outputting milling files that is capable of understanding these differences and changing things accordingly - not really relevant for our application but for high end tool making it can make significant improvements.
     
Loading...

Share This Page