510,001 active members
3,965 visitors online
Register for free
Login
IndustryArena Forum > CAM Software > Mastercam > Mastercam Planes
Results 1 to 11 of 11
  1. #1
    Registered
    Join Date
    Oct 2009
    Posts
    54

    Mastercam Planes

    Hello All,

    I am trying to figure what plane to use for machining a part with 45 degrees chamfer.
    But whatever I change the plane I always get this

    G0 G54 G90 X0. Y0. C90. B-45. S3500 M3

    C90 AND B-45. OK with B-45 but c i think it shouldnt change.

    But any plane i change the GNOMON i get the same.

    Any clues

    Thank you

  2. #2
    Registered
    Join Date
    Mar 2005
    Posts
    22

    Re: Mastercam Planes

    We need more information. Are you on a 5 Axis machine? Version of Mastercam? Can you Share the part file or at least a picture or print? Do you want to cut your 45 degree face normal to the face "side cutting" or face cutting with the end of the endmill?

  3. #3
    Registered
    Join Date
    Oct 2009
    Posts
    54

    Re: Mastercam Planes

    Yes the machine is 5axis MAXIMA from cms with Fanuc 18i-mb5 control.Mastercam 2018. (I had the same problem with x9). I want face cutting with the end of endmill.
    Please find ttached 3 files, mastercam toolpath. nci and nc.

  4. #4
    Registered
    Join Date
    Mar 2005
    Posts
    22

    Re: Mastercam Planes

    Can you post your file as 2017 mastercam? I'm still on that. If not export it as a parasolid and make a screen shot with where you are setup and I"ll program it in 2017 so you can see how it's done. thanks

  5. #5
    Registered
    Join Date
    Oct 2009
    Posts
    54

    Re: Mastercam Planes

    Thanks for your help,
    please find the file attched as 2017 mastercam. Please note setup is different as my original 2018.
    Attached Files Attached Files
    • File Type: rar T.rar (32.5 KB, 3 views)

  6. #6
    Registered
    Join Date
    Mar 2005
    Posts
    22

    Re: Mastercam Planes

    You need to create two planes. I named the main plane 5 AXIS START. You need to set your first planes WCS to what every point you want to setup off of. Next you need to create a plane facing the chamfer you want to machine. This plane I named 5 AXIS CHAM. You must set the new planes WCS to the same WCS point of the base plane (5 AXIS START). Now set the = to your base plane and then set your C plane and T plane to the second plane 5 AXIS CHAM. Once you do that set your view to the tool plane. Now you can program the chamfer surface like any 3 axis plane but when it posts it will be in 5 Axis.

    Attachment 365100

  7. #7
    Registered
    Join Date
    Mar 2005
    Posts
    22

    Re: Mastercam Planes

    Click image for larger version. 

Name:	POS1.jpg 
Views:	2 
Size:	27.3 KB 
ID:	365102
    Click image for larger version. 

Name:	POS2.jpg 
Views:	1 
Size:	27.7 KB 
ID:	365104
    Click image for larger version. 

Name:	POS3.jpg 
Views:	1 
Size:	26.7 KB 
ID:	365106
    Click image for larger version. 

Name:	POS4.jpg 
Views:	1 
Size:	41.2 KB 
ID:	365108

  8. #8
    Registered
    Join Date
    Oct 2009
    Posts
    54

    Re: Mastercam Planes

    Many many thanks, I will review and I get back to you.
    Just a quick question. doesnt have the new planes to have the same origin as wcs? (origin is bottom right corner) planes seems to be on the center.

  9. #9
    Registered
    Join Date
    Mar 2005
    Posts
    22

    Re: Mastercam Planes

    Yeah I just started over with your file. It doesn't matter where you setup your WCS, as long as your secondary plane is set at the same WCS point as your base plane. It could be the corner if you want just set them both the same.

  10. #10
    No posers
    Join Date
    Apr 2008
    Posts
    1574

    Re: Mastercam Planes

    Quote Originally Posted by platonas1 View Post
    Many many thanks, I will review and I get back to you.
    Just a quick question. doesnt have the new planes to have the same origin as wcs? (origin is bottom right corner) planes seems to be on the center.
    I think I know exactly what you are asking. I've struggled with this for a bit in the two different CAM systems I use. I believe the origin for your "tilt" planes (T/C) makes no difference in the posted code. The post will look at your machine's axis combinations and choose the correct tilt combo (B and C in your case) and all the calculations will come from the WCS origin using the T/C plane as a reference. That is the short (and not quite accurate) answer I've discovered.

    The way you set your T/C plane origins DO have an effect on your Z depths in the toolpath dialogs that use that T/C plane. For example, if the origin of the T/C plane in the pictures above was actually on that angled surface, the Z cut depth in the Linking Parameters page (in absolute) would be zero. If the origin of the T/C plane was at the WCS, the Z depth (in absolute) is going to be some positive distance.

    There also may be some consequences of the rotation (about Z) of your T/C plane. I haven't experimented as much with this but in general I make sure I rotate the T/C plane to what I think is the "correct" rotation. The machine's axis combinations might come in to play here, I'm no sure.
    -------------------------------------------------------------------------------------
    Mastercam X9/2017 Multiaxis for SolidWorks - Bobcad V29 3ax Pro 4ax Std.

  11. #11
    Community Moderator cadcam's Avatar
    Join Date
    Apr 2003
    Posts
    3533

    Re: Mastercam Planes

    He is using the wrong post kinematics of the machine. this is a A and C axis. Is this machine a Head < Head setup? as setting up the angle in 3+2 for this is easy. but if you are running the wrong machine def and post it may output different for sure. With a solid as show in you sample picking the gnomon and the face will set the Z in one click. you may need to swing the X or Y based on the machine kinematics.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

Similar Threads

  1. Planes by Normal
    By FMJ in forum Mastercam
    Replies: 0
    Last Post: 02-05-2013, 08:38 PM
  2. DXF on different planes ?
    By SScnc in forum Mastercam
    Replies: 3
    Last Post: 11-23-2010, 10:32 AM
  3. Help me please.......Planes or......
    By Radosl81 in forum Mastercam
    Replies: 4
    Last Post: 11-30-2009, 04:28 PM
  4. Planes?
    By dpark1 in forum Solidworks
    Replies: 5
    Last Post: 09-26-2009, 02:25 PM
  5. Do like R/C planes???
    By CNCadmin in forum Hobby Discussion
    Replies: 17
    Last Post: 07-30-2006, 12:17 AM

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
  •