Page 3 of 5 FirstFirst 12345 LastLast
Results 21 to 30 of 44

Thread: Vacuum Film Technique - A Quick Explanation

  1. #21
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,986

    Default

    Ed,
    I'd try slowing lightening the chipload - or bite that each flute takes per revolution of the spindle/router. You can do this a few ways...

    1) Increase RPM
    2) Reduce Move Speed
    3) Use a 2 or 3-flute spiral-O (Onsrud 65-624 or similar)

    You should put your safety glasses on (with side shields!) and get in there and observe what is going on as the parts are being cut. Are they lifting? If so, and you have reduced chipload without melting, it could be that you either don't have enough vacuum pressure or that the helical flutes of the tool are working against you - causing lifting. ANY vibration from parts lifting even a little bit, will degrade the cut quality. Parts should NOT be moving if you are using the technique & materials I outlined above. Substitutions for other products or methods will give varying results.

    If the spiral tools are lifting parts & you've done all you can do, try a 2-flute straight-O tool, which will leave chips in the kerf, aid hold down and still give a decent cut. I would not advise using straight flutes on plastic over 1/4" though, because you really want to get those chips out of there.

    Reduction in cut quality is in most cases, directly associated with worn pinions and dry gear racks...You'll also want to check the machine under power, not moving, by grabbing every axis and push/pull - listen and feel for slop in each axis. Really shake everything and listen for the tell tale 'ticking' of slop. I am not talking about the slight ticking that you hear from a 7.2:1 gearbox - this is normal. Check the v-rollers...Clean each and every rail with a scotch pad - every little bump in the rail will transfer to your cuts.

    You should be running those small bits between .5 & 1 IPS and 18,000 RPM. If you are not, your chipload is probably too high.

    -B
    High Definition 3D Laser Scanning Services - Advanced ShopBot CNC Training and Consultation - Vectric Custom Video Training IBILD.com

  2. #22
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,633

    Default

    I have been cutting a lot of lexan lately. some really thin .03 stuff. but even with a custom vac setup and very strong vac these things move a bit. a simple solution was spraying the vac bed with contact adhesive. that would lock them in place.

  3. #23
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,986

    Default

    Steve,
    You seem to have missed the point of the technique...Spraying glue right on the bleeder is a sure way to seal it and completely defeat your efforts...

    -B
    High Definition 3D Laser Scanning Services - Advanced ShopBot CNC Training and Consultation - Vectric Custom Video Training IBILD.com

  4. #24
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,633

    Default

    I had holes for the vacuum. but even with the very strong vac the lexan would jiggle. so the spray made things non slip.
    I just had to cut 8 more sheets so I just vacced down a piece of 1" mdf flattened it and used the spray on both sides. but this only worked because of hte size of the pieces and that they were so thin.
    I am waiting for the pressure foot and then I can dump the spray all together.

  5. #25
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,633

    Default

    I forgot I had to cut 4 full sheets of thin lexan and nothing on hand. so I just sprayed the spoilboard with 77 and used my vac too no parts slipped though I used the spoilboard afterward without a problem it was nicer to surface it first.
    this is a messy fast solution but it does work for thin plastics.

  6. #26
    Join Date
    Apr 2005
    Posts
    65

    Default

    I will try cutting again and go a bit slower. I was at 18K rpm (my max) and 2" per sec as per the folks at Onsrud for 3/16 polycarb. And again, my true straight cut (straight move in X) was pretty flat and smooth. It was the angled and arched cuts that were bad. The was no re-melt which is good. I have had problems with that in the past, mainly with acrylic. I'll also make sure everything is tight (although I do this routinely). For what it's worth, my tool isn't likely to have anything "worn" on it since it get so little use.

    Also, what type of pressure foot are you referring to? Is that like a roller hold down of sorts?

    Thanks!

  7. #27
    Join Date
    Apr 2005
    Posts
    65

    Default

    Another thought!

    I reviewed comments on polycarb cutting about 10 posts down. I looked at my geometry in Artcam (insignia) and the angle and curves looked segmented. I just always assumed that's a graphics limitation. Could I be creating lines instead of arcs? Although, my angled line looks segmented as well. Only my straight line in X looks truly smooth on the screen.

    As mentioned previously, I am creating in Acad LT, importing .dxf into Artcam, then tool path using arcs/mm.

    Once again, suggestions are appreciated.

  8. #28
    Join Date
    Mar 2009
    Location
    Eastern Delaware
    Posts
    315

    Default

    Ed;
    I don't use Autocad LT, but some designers I cut for do. I have seen some lines that I think they intended to be arcs come into Aspire as segmented sections. I replace them with arcs or Bezier curves. On other drawings I believe they have been arcs when they imported, so I am guessing it depends on how Autocad is setup to export or save a file?

  9. #29
    Join Date
    Sep 2006
    Location
    cnc routing, portland or
    Posts
    3,633

    Default

    I have been only using straight bits for the thinner plastic polycarb for sure. the smaller the bit the better. usualy the shavings don't reweld. I cut 8k at most. I was cutting some .03 lexan yesterday with a 1/16" onsrud 1f straight bit at 3ips and 10 or 12k. I used spray adhesive on both sides because the parts were small.
    52 parts per 2x4 sheet.
    Now I cut a full sheet of .5 lexan using a 1/4" o flute upcut in two passes at 1.5ips and the last pass was really vibrating. the peices were about 14x18 and the vac could not hold them down. I think this is a real issue with lexan it seems more grabby then most other plastics. so the straight bit really helps in through cuts.
    Widget works if he ever gets his rear in gear (hey just joking) is coming out with a great (from what I have heard) pressure foot that will let us cut parts down to .25 square.

  10. #30
    Join Date
    Apr 2005
    Posts
    65

    Default

    Steve, I think you're right about the particulars of Lexan. I know it's considered a "soft" plastic to cut, even though it's "tough as nails." I think that does make it grab more. Also, when I've cut .5" lexan, and I remove a considerable amount of material, the sheet seems to curl (stress relieve?) up and off the table,,,,,,bye bye vacuum.

    I am going to try .125 Lexan on Monday and see if I get acceptable results over the .187 I've been playing with.

Similar Threads

  1. 2 sided technique
    By ADAPT_Shop-Brady in forum Techniques for Cutting, Drilling, Machining
    Replies: 0
    Last Post: 09-15-2016, 06:01 PM
  2. Gold Lettering Technique
    By joe in forum Sign Making
    Replies: 11
    Last Post: 12-31-2015, 12:18 PM
  3. Shocking Technique
    By Mayo in forum Techniques for Cutting, Drilling, Machining
    Replies: 10
    Last Post: 01-28-2015, 12:58 PM
  4. Quick and cheap vacuum setup?
    By ron_churches in forum ShopBotter Message Board
    Replies: 10
    Last Post: 08-16-2011, 01:33 PM
  5. Easy Hold Down Technique
    By joe in forum ShopBotter Message Board
    Replies: 12
    Last Post: 04-02-2009, 01:41 PM

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
  •