G-code editor - Page 2


Page 2 of 3 FirstFirst 123 LastLast
Results 13 to 24 of 27

Thread: G-code editor

  1. #13
    Member
    Join Date
    Sep 2017
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Thanks! That's the type of routine I was thinking about. My other "brute force" method was going to be writing a formula in Excel. It'd be pretty simple in Excel, but your G-code routine is the way to go.

    Bruce



  2. #14
    Member
    Join Date
    Jun 2012
    Location
    usa
    Posts
    151
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Fusion 360 CAM can use patterns, so you would only need to create the toolpath for 1 tooth, then pattern the rest.



  3. #15
    Member kstrauss's Avatar
    Join Date
    Apr 2013
    Location
    Canada
    Posts
    1438
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    How would patterns help if he is using a gear cutter? For the size gears that he wanted to cut a 0.5mm endmill would be too large.



  4. #16
    Member
    Join Date
    Jun 2012
    Location
    usa
    Posts
    151
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    What difference would it make whether it's a gear cutter or an endmill? You create the gcode path for 1 tooth, then repeat for each tooth.



  5. #17
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    1734
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    My cam system post processor generates simple repeated code. The tool path code is repeated for each tooth and the only change is 4th axis move.
    G-code editor-geartoolpaths-jpg



  6. #18
    Member
    Join Date
    Dec 2003
    Location
    East Anglia,England
    Posts
    388
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    If you operate in the world of Windows, wordpad works.In a Linux environment I use mousepad.



  7. #19
    Member kstrauss's Avatar
    Join Date
    Apr 2013
    Location
    Canada
    Posts
    1438
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Probably my lack of knowledge of Fusion is showing but setting up a 4-axis job to simply move a cutter parallel to the rotary axis and at the z-height of the rotary's centre line seems unduly complicated.



  8. #20
    Member
    Join Date
    Sep 2017
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Here are a couple of the gears I've made using a conventional dividing head. One's a 50-tooth gear, others are 10/75 teeth. I've got the gear cutters for all three though the 10-tooth is using whatever the smaller number of teeth you can get with a cutter, something like 12 or 13 teeth. Not the correct cutter as they don't make one for 10 teeth, but as close as I could get. Use is in a toy, so not Space Shuttle tolerances.

    I'll be learning Fusion this winter. I'm thinking that it's really a simply process for conversational G-code since it's just making a pass, returning to the original position, rotate the 4th axis, then repeat. I've got the math down on determining the gear blank OD, diametral pitch, tooth whole depth, etc. Nice to have some canned math equations (i.e. whole depth = 2.157 / P) so I don't have to manually calculate the coordinates for each different gear.

    Tips below will help immensely. I was unaware that G-code allowed variable names to be assigned. I can see writing a number of canned routines, like cutting gears, tension/compression tapping, etc. that can be added into other pieces of the CAD design.

    For example, might be easier to draw the shape of a part in Fusion, put in the holes, but do the tapping after the fact from a G-code routine calling up Tormach's recommended tension/compression G-code routine. I've got a number of thread mills also, so can go that route too. Just don't understand (yet) how Fusion would know to make a 1/4"-20 hole via a thread mill or a T/C head with a tap.

    Thanks again for the help,

    Bruce


    G-code editor-cutting-p50s-jpg
    G-code editor-cv-cw-jpg

    Attached Thumbnails Attached Thumbnails G-code editor-cv-cw-jpg   G-code editor-cutting-p50s-jpg  


  9. #21
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3718
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Quote Originally Posted by BGHansen View Post
    I've got a number of thread mills also, so can go that route too. Just don't understand (yet) how Fusion would know to make a 1/4"-20 hole via a thread mill or a T/C head with a tap.

    Thanks again for the help,

    Bruce
    Fusion has a thread milling function built in, I use it all the time.

    Jim Dawson
    Sandy, Oregon, USA


  10. #22
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    1734
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Quote Originally Posted by kstrauss View Post
    Probably my lack of knowledge of Fusion is showing but setting up a 4-axis job to simply move a cutter parallel to the rotary axis and at the z-height of the rotary's centre line seems unduly complicated.
    In sprut I use a standard 2d operation that follows an edge on the model. The example above shows the actual gear model, but I don't use that for the operation setups.
    Quick summary.
    1) I draw the gear blank model to the exact exterior root diameter of the gear. ( o.d. = (n+2)/p n= number of teeth)
    2) I put a single line centered on axis on the surface of blank model. (in pic below)
    3) Import model into sprut and position on 4th axis.
    4) Defined a arbor saw as the cutter with the center of the outside cutting edge to be contact point on tool. (important) outside diameter set to the gear cutter diameter measured at bench and used for that gear.
    5)Setup a standard 2d operation to follow the line on the gear blank model.
    6) multiply the 2d operation tool path by axis "A" set the multiply number to the number of gear roots or teeth -1 on the model.
    7) Compile code and check simulation. (shown in above post)

    I found gear cutter diameters to vary slightly from cutter to cutter. And user needs to keep this in mind when setting up cam operations.

    The manual method shown in post above, the cutter is centered and touched off . Then depth of cut (w) = 2.157/p is used for the cutter passes. Touching off the cutter would reduce error from cutter diameter differences that causes problems in cam setups.

    G-code editor-rootlinesprut-png


    I often draw threads and gear teeth because the models look better but I don't use them in cam operation setup. Thread milling, tension compression tapping are all simple operations to have preset for every type and size standard or custom in your cam software. Then user can load desired thread operation select model features, compile and your done. Super fast in cam software to do after you learn the process. And most cam software allows user defined ops. So complete sets of custom operations can be preset (drill pilot, drill size, tap) and saved for easy setup on all projects. This minimizes the time to setup and complete a complex model.

    Last edited by mountaindew; 09-14-2019 at 08:27 AM.


  11. #23
    Member
    Join Date
    Nov 2012
    Location
    United States
    Posts
    317
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Touching off the cutter would reduce error from cutter diameter differences
    I imagine you could also do this with different tool numbers for different cutters in the CAM, or by using tool wear offset in the controller?



  12. #24
    Member mountaindew's Avatar
    Join Date
    Nov 2007
    Location
    earth
    Posts
    1734
    Downloads
    0
    Uploads
    0

    Default Re: G-code editor

    Quote Originally Posted by jwatte View Post
    I imagine you could also do this with different tool numbers for different cutters in the CAM, or by using tool wear offset in the controller?
    I define the tools in sprutcam and pp the same. Each cutter has a tool number and description and carefully measured. I just made note above because the ease of using published numbers in cam and pp then wonder what went wrong. Chase it back to one or 2 cutters in set with different Diameters. You would not notice this if you touched off , zeroed and cut to depth



Page 2 of 3 FirstFirst 123 LastLast

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
  •  


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

G-code editor

G-code editor

G-code editor