584,802 active members*
4,769 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > BobCad-Cam > Circle pockets always under my specs in cad, but using mach circle wizard perfect?
Results 1 to 17 of 17
  1. #1
    Join Date
    Jan 2013
    Posts
    43

    Circle pockets always under my specs in cad, but using mach circle wizard perfect?

    Hi Guys, I have a question if anyone could point me in the right direction.

    Example:

    If I design a 30mm pocket in bobcad and go out on my mach 3 machine and cut it it will be about .15mm smaller than 30mm. I though maybe it was backlash so I went through and checked and tested etc.... and that was not the issue. Finally someone told me to use the circle wizard in mach3 and if that works it is something in the cad/cam. So I did a circle 30mm in mach3 circle wizard and it was perfect. So I guess this means the machine is correct, but what would it be in Bobcad, maybe a setting I am missing?

    Thanks so much guys

  2. #2
    Join Date
    Mar 2003
    Posts
    35538
    So I guess this means the machine is correct........................
    That's a pretty big assumption.
    Cut two 30mm pockets in BobCAD, one climb cut and one conventional cut. See if they are the same size., or, program the same circle in BobCAD trhat you did in Mach3, being sure to cut in the same direction. They'll probably be the same.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  3. #3
    Join Date
    Jul 2013
    Posts
    32
    If you were brand spanking new to Bobcad, I would say you defined a Side Allowance value but then didn't define a finish tool. The only real possibility that comes to mind is that it might be something in your post processor - maybe you aren't keeping enough decimal points in your G-code. I pulled these parameters from my post processor.

    414. Number of decimal places for metric numbers ? 3
    415. Number of decimal places for english numbers? 4
    425. Number of decimal for angles? 2

    I'm assuming your Mach 3 option doesn't produce G-code but just runs the operation - sorry I'm not familiar with it? I'd say post your G-code here for a simple circle - I'm going to assume it is going to show that circle path is short by .15 mm. Another possibility is how your setup might be interpreting curves - whether it be arcs or lines.

  4. #4
    Join Date
    Jan 2013
    Posts
    43
    Thanks for the suggestions.

    I did cut the circle the same in bobcad and in mach3 circle wizard, (same direction climb), I am not a master with Bobcad but I know my way around fairly well to use often with mostly no issues.

    Also It is not a finish allowances left out

    I looked at the Bobcad G code and it is showing the correct movements to make a 30mm circle.

    I am wandering if it is a circle or arc setting somewhere like rfenn mentioned?

    Thanks so much for the replies

  5. #5
    Join Date
    Apr 2009
    Posts
    3376
    Compensation setting??
    Upload a .bbcd,will have a look.

  6. #6
    Join Date
    Jan 2013
    Posts
    43

    files

    Here is the bbcad file zip and gcode.

    Thanks so much for the help

  7. #7
    Join Date
    Oct 2004
    Posts
    832
    You seem to have a side allowance of 1mm on the finish pass.
    Hood

  8. #8
    Join Date
    Jan 2013
    Posts
    43
    I do have a side allowance , but I also have a finish cut for that.

  9. #9
    Join Date
    Oct 2004
    Posts
    832
    What version of BobCAD are you using as I see a 1mm side allowance on your finish pass. I am using V26.
    See screenshot.
    Hood
    Attached Thumbnails Attached Thumbnails ScreenHunter_04 Feb. 05 12.15.jpg  

  10. #10
    Join Date
    Jan 2013
    Posts
    43
    I'm Am using V25, and Yes I know I have a 1mm side allowance, but it is cut with the finishing pass. So that's not the issue. If you look at the G-code you will see the finish pass operation that cuts the 1mm allowance?

    Again the circle is about .15mm smaller than 30mm when you measure after its machined.

  11. #11
    Join Date
    Oct 2004
    Posts
    832
    Ok that screenshot above is the finish pass, so there is 1mm set there. HOWEVER this is in V26 and I have noticed some files do not import correctly from previous versions so that is likely why it is showing the 1mm allowance in the finish pass.
    Will open in V25 and see.
    Hood

  12. #12
    Join Date
    Oct 2004
    Posts
    832
    Ok opened in V25 and it looks fine, also produced code with my PP and it ties in with yours and is correct. If you look at the finish it is calling for a rad of 10.238mm so double that and add your cutter dia and you get
    10.238 + 10.238 + 9.525 = 30.001mm dia it should cut.
    So code is not your problem as far as I can see.

    Hood

  13. #13
    Join Date
    Jan 2013
    Posts
    43
    Thanks ,yea Im not sure whats going on. Maybe some arc setting somewhere or something?/ I don't know....., the G code like you said is correct just don't know why using the simple mach3 circle pocket wizard I can get results but when I use my Bobcad Gcode I do not?

    Thanks again for the help


    Quote Originally Posted by Hood View Post
    Ok opened in V25 and it looks fine, also produced code with my PP and it ties in with yours and is correct. If you look at the finish it is calling for a rad of 10.238mm so double that and add your cutter dia and you get
    10.238 + 10.238 + 9.525 = 30.001mm dia it should cut.
    So code is not your problem as far as I can see.

    Hood

  14. #14
    Join Date
    Oct 2004
    Posts
    832
    Machs pocket wizard uses R instead of IJ but cant see that being an issue.
    Are you using the same tool number and same feeds and speeds in the wizard as in BobCAD?
    Hood

  15. #15
    Join Date
    Jan 2013
    Posts
    43
    Yep, same tool, same speeds, same direction and everything.




    Quote Originally Posted by Hood View Post
    Machs pocket wizard uses R instead of IJ but cant see that being an issue.
    Are you using the same tool number and same feeds and speeds in the wizard as in BobCAD?
    Hood

  16. #16
    Join Date
    Jan 2013
    Posts
    43
    Got it, thanks so much for all your help. It was indeed tool deflection. As I had a deeper cut programmed in Bobcad than in the Machwizard.

    I feel like a dork..lol Thanks again to all of you

  17. #17
    Join Date
    Apr 2009
    Posts
    3376
    If you buy from un-reputable sellers on E-Bay,,EM will be off dimensional size that much.

Similar Threads

  1. circle cutting wizard
    By billmiller in forum Mach Wizards, Macros, & Addons
    Replies: 4
    Last Post: 03-26-2016, 11:37 AM
  2. CNC not cutting perfect circle
    By nambass in forum DIY CNC Router Table Machines
    Replies: 20
    Last Post: 01-29-2014, 11:52 PM
  3. Newfangled Circle wizard problem
    By MFchief in forum Tormach Personal CNC Mill
    Replies: 7
    Last Post: 02-23-2012, 06:27 AM
  4. mach 3 wizard circle cutting
    By billmiller in forum Shopmaster/Shoptask
    Replies: 1
    Last Post: 05-28-2010, 11:02 AM
  5. The Perfect Circle - Need Help
    By ScoobyDoo in forum FeatureCAM CAD/CAM
    Replies: 11
    Last Post: 01-17-2007, 11:41 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
  •