CNC Cutting Acrylic and Perspex

Results 1 to 11 of 11

Thread: CNC Cutting Acrylic and Perspex

  1. #1
    Registered
    Join Date
    May 2007
    Location
    UK
    Posts
    25
    Downloads
    0
    Uploads
    0

    Default CNC Cutting Acrylic and Perspex

    Hi all,
    I'm sure this is a common question but I can't find exactly what I'm after on the forum. It concerns cutting 3 - 5mm thick Acrylic or Perspex, I get a problem with melting but I have researched it here.

    I'm a new user with a Zenbot CNC, 24 x 16 bed. I bought a Kress 1050 Motor for it and a selection of small bits. I understand that I should use a single flute cutter to get a clean cut with a slow speed. My machine will run from 5000 to 25000, so I assume 5000 would be best. What I need to know with this cutter (3mm single flute) at 5000 what feed rate should I use. Is there a formula I can use? Any advice would be appeciated.

    Regards
    Joe Lavery.

    Similar Threads:


  2. #2
    Member
    Join Date
    Feb 2006
    Location
    USA
    Posts
    198
    Downloads
    0
    Uploads
    0

    Default

    use dishwashing detergent as a lube and coolant I mix with a little water then smear on the plate to engrave on it

    In the words of the Toolman--If you didn't make it yourself, it's not really yours!
    Remember- done beats perfect every time!!


  3. #3
    Registered rich909's Avatar
    Join Date
    Feb 2011
    Location
    U.S.A.
    Posts
    109
    Downloads
    0
    Uploads
    0

    Default Plastic cutting formula

    Hi Joe --

    Quote Originally Posted by Joe Lavery View Post
    <snip>
    My machine will run from 5000 to 25000, so I assume 5000 would be best. What I need to know with this cutter (3mm single flute) at 5000 what feed rate should I use. Is there a formula I can use? Any advice would be appeciated.
    <snip>
    I've been using an unscientific 'test cut' approach in determining the best speed/feed for materials, but there are a couple of formulas that you could use.

    1) IPM = IPT x No. Teeth x RPM
    2) SFM = .262 x Diameter (inches) x RPM or RPM = 3.82 x SFM / Diameter (inches)

    In the first formula, IPM is Inches Per Minute, of course, and IPT refers to the Inches of material removed Per Tooth. In the second, SFM refers to the surface feet per minute which is the speed at which the cutting edge of the tool is striking the material.

    For your purposes I'd guess the first formula might be most useful. I have plugged in my set up for 1/8" acrylic sheet and the formula gives a very close result to what I normally run. The only value you may not have is the IPT Spec, which might be available from your material supplier. If not, I have found that .004" to .015"/tooth is the general range for Acrylic sheet.

    Plugged in to what you are using you would have:
    5000 * 1 * .015 = 75 IPM ...for the heaviest recommended cut or

    5000 * 1 * .004 = 20 IPM ...for the lightest.

    In my trial and error method, I have found 50 IPM seemed to work best with an IPT of .0138 while the formula suggests 69 IPM. I will give it a try on my next job and see.

    HTH!

    --Rich



  4. #4
    Registered
    Join Date
    May 2007
    Location
    UK
    Posts
    25
    Downloads
    0
    Uploads
    0

    Default Confused

    Hi Rich,

    Firstly thanks for such an informative answer, some of the accronyms found on the forum were confusing me.

    While I understand the points and suggestions you make, I don't understand the final analysis where you give an example: i.e.

    Plugged in to what you are using you would have:
    5000 * 1 * .015 = 75 IPM ...for the heaviest recommended cut or

    5000 * 1 * .004 = 20 IPM ...for the lightest.


    My (possibly flawed) logic would be that the heaviest cut would be the slower of the two; can you clarify this for me

    As far as using a formula is concerened, it's going to be more difficult than I thought. Mainly because the cutters I have came with the machine; so I have no way of finding out the IPT spec. I think I may be resigned to the same "test cut" approach that you use.

    Incidentally when cutting say a 3mm (1/8") sheet at 5000 PRM and 50 IPM, how many passes would you take to cut it?

    Thank you once again Rich, your help is much appreciated.
    Kind regards

    Joe.



  5. #5
    Registered
    Join Date
    Oct 2005
    Location
    Australia
    Posts
    2392
    Downloads
    0
    Uploads
    0

    Default

    Hi Joe, brand new cutters are essential!

    I use HSS (high speed steel) cutters for acrylic, they are a little sharper than carbide and last for a LONG time as they only get used in acrylic.

    For cutting 3mm sheet I would cut it with a 5mm HSS endmill, 3 flute, with 2 or 3 passes in depth and about 10mm to 15mm per second feedrate, between 7000 and 11000 RPM, and usually leaving a small 0.15mm skin on the bottom so the pieces stay attached in.

    I think the bulk of your problem is blunt tools, they may have been used on woods or metals. Get some good brand name virgin HSS endmills and you will be very happy.



  6. #6
    Registered rich909's Avatar
    Join Date
    Feb 2011
    Location
    U.S.A.
    Posts
    109
    Downloads
    0
    Uploads
    0

    Default Fromula follow-up

    Hi Joe --
    Quote Originally Posted by Joe Lavery View Post
    <snip>
    While I understand the points and suggestions you make, I don't understand the final analysis where you give an example: i.e.

    Plugged in to what you are using you would have:
    5000 * 1 * .015 = 75 IPM ...for the heaviest recommended cut or

    5000 * 1 * .004 = 20 IPM ...for the lightest.


    My (possibly flawed) logic would be that the heaviest cut would be the slower of the two; can you clarify this for me
    <snip>
    I think of the heavier cut in terms of the Inches of material removed Per Tooth (IPT), so that .015" of material removed is a heavier cut (done at higher speed) than .004".

    <snip>
    Incidentally when cutting say a 3mm (1/8") sheet at 5000 PRM and 50 IPM, how many passes would you take to cut it?
    <snip>
    I normally use 9-passes to profile a 1/8" piece, with tabs to hold pieces together, and using a 0.0138" pass depth. Looking at this with you now ...I'm thinking a pass depth of 0.0144" makes more sense. Based on the Zenbot's 139 full steps to the inch, each one is 0.00719", and two full steps would be 0.01438", and still a fairly light cut. Either one- step or two-step pass depth are within range for the IPT on acrylic sheet for your Zenbot.

    Actually, I think Roman is right. You will never get good results with dull cutters, so that is the first priority.

    HTH!

    --Rich



  7. #7
    Registered
    Join Date
    Sep 2011
    Location
    CHINA
    Posts
    49
    Downloads
    0
    Uploads
    0

    Default

    Where you buy the machine?You should ask the man who sell these products to you,They are the best understanding man of this product .My company is MORN,if you need something like:CNC router/Laser engraving /Laser cutting machine/ECT,please contact me

    http://www.morntech.com/: Laser engraving machine , CNC router


  8. #8
    Registered
    Join Date
    May 2007
    Location
    UK
    Posts
    25
    Downloads
    0
    Uploads
    0

    Default

    Thanks everyone for the advice, it's much appreciated.

    Incidentally I have quite a range of cutters which are all brand new. The guy who originaly bought the ZenBot didn't enev power it up. So the cutters have never been used.
    I have ordered some single flute cutters 2 and 3 mm which I'm told don't cause as much heat.
    In any event I have a large supply of Acrylic to test with, so I'll use this advice and see how I get on.

    Best regards
    Joe.



  9. #9
    Registered
    Join Date
    Oct 2005
    Location
    Australia
    Posts
    2392
    Downloads
    0
    Uploads
    0

    Default

    Hi Joe, if in doubt use lighter cuts than the tool makers recommend and possibly a squirt of water from a perfume bottle or gardening mister bottle. The lighter cut generates less heat in total, and also your machine is smaller and less rigid than many large commercial routers the tool makers specify for their feedrates etc.

    Also, just because the tools are new doesn't mean they are sharp. Many tools especially in sets are garbage and were never sharp when new. Likewise Dremel "bits" which are usually "bits of garbage". I do a lot of acrylic and use mainly 4-flute and 3-flute HSS endmills designed for metalwork, from a top brand name cutting tool maker. They work very well.



  10. #10
    Registered
    Join Date
    May 2007
    Location
    UK
    Posts
    25
    Downloads
    0
    Uploads
    0

    Default

    Hi all,

    Thanks very much for all your help. I sucessfully cut and engraved a clock face today, it's not perfect and I probably couldn't repeat the process exactly as I did, but it's a good start.

    At least I didn't break the cutter, or destroy the acrylic I used.

    Best regards
    Joe.



  11. #11
    Registered
    Join Date
    Dec 2011
    Location
    Finland
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default Throwing in my 2 cents

    Hello,

    I happened to stumble upon this thread and decided to say thoughts of my own as just last week I started to work with Perspex!

    We usually work with range of plastics and use airflow as coolant. It is usually sufficient depending on the working speeds. Thus I didn't have any problem with melting because of the airflow from the nozzle.

    The first attempt failed as there was some shattering because of too large step i.e. too much stuff for the teeth to work with. I use 4 mm in diameter, 2 flute HSS cutters. I dropped the Z-step to 0.5 mm millimeters with 14000 RPMs and 180mm/min feed. Sounds rough but worked (on saving time too) and the finish was suprisingly good.

    The 8 mm Perspex sheet was on a MDF-sheet placed on a suction table. The suction is powerful enough to suck the acryl tightly through the MDF. This enables to machine through the acryl sheet with no need to finish by hand. Theres always danger of shattering in that scenario.


    This was just some thoughs on the subject, still working on the optimal speeds.. Awesome and very helpful forum btw!

    Erno Pystynen
    Micromechanic



Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

CNC Cutting Acrylic and Perspex

CNC Cutting Acrylic and Perspex