Page 2 of 3 FirstFirst 123 LastLast
Results 11 to 20 of 23

Thread: Machining both sides of material

  1. #11
    Join Date
    Dec 2008
    Location
    Diamond Lake, WA
    Posts
    1,605

    Default

    Like Steve says. I cut 4" circles and ovals from 1/4" MDF all the time and take the parts to the router table and round the edges while the next sheet is cutting. I do the same thing with larger circles, ovals and football shapes I cut from 1/2" MDF. I thought about trying it on the CNC but figured I could do it faster at the routertable then dealing with the flip operations at the CNC.

    To accomplish flip operations, you need to create an exact mirror image of your vectors. You also have to have an EXACT size for your material. And I mean dead on. The original side vectors should be centered in the material. The flip side with the mirrored vectors should also be centered in the material. Then you need to have a registering system on your table that enables you to position the material in exactly the same position when you flip the sheet. For those that do flip operations with SBLink for cabinet parts, we deal with this all the time.

    I'm about to cut several dozens sheets of sign letters on laminate on MDF substrate using flip operations to stud mounting holes and write sign numbers on the back (using Widgetworks pen system), them flipping the whole sheet over, beveling the letter edges and cutting out the letters from the front side. I have indexing pins (SBLink) on my CNC table that enable me to register the sheet in exactly the same spot for the flip operations. It is time consuming and tedious but I have about 800 letters to cut out ranging is size from 1.5"x1.5" square up to letters 52" tall.
    Don
    Diamond Lake Custom Woodworks, LLC
    www.dlwoodworks.com
    ***********************************
    Life is not a journey to the grave with the intention of arriving safely in one pretty and well preserved piece; But to skid in broadside, thoroughly used up, worn out, bank accounts empty, credit cards maxed out, defiantly shouting "Geronimo"!

    If you make something idiot proof, all they do is create a better idiot.

  2. #12
    Join Date
    Mar 2011
    Location
    Louisiana
    Posts
    53

    Default

    Thanks everyone for your suggestions. After testing out several ideas we've decided to approach it per Steve and Don's suggestions...half on the machine half manually. We now realize what is involved with successfully machining both sides of the stock with the profile that we're trying to achieve...ehh it has been an aggravating process but we've learned a great deal.

    Thomas it's funny you mention that because we just thought about the prospect of running some sort of convex edging router bit on the circles...but as you said, it's probably more time consuming in setup than it's worth.

    Thanks again everyone,

    -Pat

  3. #13
    Join Date
    Jun 2012
    Location
    Philadelphia
    Posts
    448

    Default

    I have done some "flip" parts, I really don't produce a large quantity of anything so I have the luxury of being able to use the bot to precut my blanks instead of needing to use a saw ahead of time. I create a vector the exact same size as my material in the same partfile my part are coming from but save the toolpath for the blank to its own cut file. I cut the blank, reposition it on the table and clamp runners to the edge of my table, when I flip the board I simply but it back up against those runners and everything comes out dandy.

  4. #14
    Join Date
    Mar 2006
    Posts
    7,830

    Default

    just thinking off the top of my head but why couldn't you elevate your part slightly off the table, cut your hole, then use a bit like this:
    http://www.magnate.net/index.cfm?eve...roup&theID=141
    Bull Nose (Half Round) Carbide Tipped Router Bit, 2 Flute
    to go to the center of your hole then then do a profile cut around the edges?
    It might be hard to toolpath but it might do it in one or 2 passes (top and bottom)
    Attached Images Attached Images

  5. #15
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,932

    Default

    If the parts could be saw sliced from round stock, I would do that first. If not, cut out the circles and put them aside. Then screw down a planed piece of 1x8 lumber to the table and machine a series of V-shaped pockets a little less than the thickness of the material in depth. Then, make yourself some cam clamps. You drop the circle/puck into the crotch of the V pocket and cinch the cam clamp against the puck. It is not going anywhere.

    You will use the vectors in software to program the machining. It should take no longer than 30 seconds to to a row of 10 pieces. Loosen the clamps, flip them over and run them again. It is safe, fast and it works. I did about 7,500 pieces just like this. It was the only way to maintain Z consistency (even .005" or so will mess up the roundover) - I got to keep all my fingers, and the quality was perfect. I programmed the tool to get out of my way after a run...It goes pretty quickly.

    There's always more than one way to skin a cat...

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

  6. #16
    Join Date
    Mar 2011
    Location
    West Chester, PA
    Posts
    37

    Default

    Brady,

    I think you are talking about putting a radius on a round "wheel".

    The OPs photos look like he's trying to put the radius on the negative or "hole". Both sides.

    Am I incorrect?

    If the goal is the latter, the recommendations about the roundover bit in the hand held router as a second operation are very good. The router base indexes on the top of the material, eliminating the "Z" error that is possible because the CNC is indexing from the rails / carriage and because your material is almost never very flat - in relative terms.

    As has been mentioned, the efficiency of the production run and the associated jigging / setup is a balancing act. If you have to make twenty of something, your setup may be diffferent from a run of several hundred.

    Sometimes the faster and better way is not the CNC. But sometimes I do it with the CNC anyway, 'cause its just so freakin' cool!

    Brent
    http://www.dcscnc.com

  7. #17
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,932

    Default

    Brent - You are correct. Not sure how I missed that one...

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

  8. #18
    Join Date
    May 2011
    Location
    Manitoba, Canada
    Posts
    79

    Default

    Most importantly your machine must be virtually perfectly in square in XY or you will never perfectly align a flip. Any out of square will basically double when you flip the piece over and no jig fixture or change of origin point or mirror image is gonna fix that. Check. Your machine for square first before getting frustrated with all the other stuff, been there done that and got the t-shirt

    Gerald

  9. #19
    Join Date
    Jan 2011
    Location
    gleason, wi 54435
    Posts
    429

    Default

    The most accurate way to flip mirror image is to use your router to machine 4 holes near each corner of the sheet into the spoilboard about 3/8 inch. Cut the first side of the material, flip the material per your mirror image program, line up the sheet over the 4 holes in the spoilboard and tap in 1/4 inch pins through the sheet and into the spoilboard (we used the broken shank from dull 1/4 inch bits). Make sure there is no play in the pins, if necessary fill the spoilboard holes with epoxy and remachine them if they get sloppy at all. You should have perfect line up every time if you follow this procedure regardless of corners not square on your material.
    Bob

  10. #20
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,932

    Default

    Quote Originally Posted by backyard_cnc View Post
    Most importantly your machine must be virtually perfectly in square in XY or you will never perfectly align a flip. Any out of square will basically double when you flip the piece over and no jig fixture or change of origin point or mirror image is gonna fix that. Check. Your machine for square first before getting frustrated with all the other stuff, been there done that and got the t-shirt

    Gerald
    Excellent point.

    Since you already have all these holes in the board, why not machine yourself 4 precise circles that fit into the holes in each corner of the board? Just pocket them into your spoilboard maybe .060" deep or so to register them with the rest of your CAD file, and use them to perfectly align the sheet on the flip? You could tag a screw in the center of each one to keep them in place when machining the 2nd side.

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

Similar Threads

  1. Machining 5"material
    By brian in forum Techniques for Cutting, Drilling, Machining
    Replies: 2
    Last Post: 01-17-2016, 09:22 AM
  2. Selecting two sides of a rectangle
    By banderson in forum ShopBotter Message Board
    Replies: 4
    Last Post: 11-03-2012, 09:42 AM
  3. Why the High Table Sides?
    By joe_dusel in forum ShopBotter Message Board
    Replies: 37
    Last Post: 05-27-2009, 05:29 PM
  4. Table sides
    By steve in forum Archives2008
    Replies: 2
    Last Post: 02-25-2008, 10:44 PM
  5. Cutting on two sides of a sheet- help
    By andrewm in forum Archives
    Replies: 8
    Last Post: 02-09-2004, 10:23 PM

Posting Permissions

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