584,841 active members*
4,316 visitors online*
Register for free
Login
Page 1 of 6 123
Results 1 to 20 of 101
  1. #1
    Join Date
    Mar 2008
    Posts
    452

    Axis orientation flips

    I am running a 4-axis tree mill... chinese wood mill system, 2.2kw 3-axis with rotary A-axis.
    Currently making pool cues and having trouble making toolpaths.
    The rotary runs down the Y-axis, so if I wanted to make a straight cut along the length of a pool cue, it would be Y+/-

    Whenever I try to create toolpaths in solidworks cam, the coord system keeps changing on me.
    I created a coord system oriented exactly as on the machine (Y-axis runs down cue, Z is up).
    But when I use that coord system or create a new one in SolidworksCam... when I run the simulation, it instead switches the length of the cue (which is the Y-axis), to Z-axis.

    What am I doing wrong?
    I have tried changing the coord system and also the plane on which the part was drawn, it does same thing every time.

    SolidworksCam Config:
    Mill Machine = 4-axis
    Post Processor = Tried 4-axis demo and also a Mori-seiki 4-axis
    Setup = Indexing set to 4-axis
    Fixture coord system = assigned as cnc machine is
    Rotary Axis = Y-axis
    0-degree position = XY plane

    Attached are two pictures, one is a screenshot showing the coordinate system used... the other shows what happens when I run a simulation.
    Why does it rotate the coordinates?
    It's supposed to be milling the face of the tapered cylinder (cue).
    Attached Thumbnails Attached Thumbnails Correct Axis.jpg   Wrong Axis.jpg  

  2. #2
    Join Date
    Jan 2013
    Posts
    474
    Quote Originally Posted by viroy View Post
    I am running a 4-axis tree mill... chinese wood mill system, 2.2kw 3-axis with rotary A-axis.
    Currently making pool cues and having trouble making toolpaths.
    The rotary runs down the Y-axis, so if I wanted to make a straight cut along the length of a pool cue, it would be Y+/-

    Whenever I try to create toolpaths in solidworks cam, the coord system keeps changing on me.
    I created a coord system oriented exactly as on the machine (Y-axis runs down cue, Z is up).
    But when I use that coord system or create a new one in SolidworksCam... when I run the simulation, it instead switches the length of the cue (which is the Y-axis), to Z-axis.

    What am I doing wrong?
    I have tried changing the coord system and also the plane on which the part was drawn, it does same thing every time.

    SolidworksCam Config:
    Mill Machine = 4-axis
    Post Processor = Tried 4-axis demo and also a Mori-seiki 4-axis
    Setup = Indexing set to 4-axis
    Fixture coord system = assigned as cnc machine is
    Rotary Axis = Y-axis
    0-degree position = XY plane

    Attached are two pictures, one is a screenshot showing the coordinate system used... the other shows what happens when I run a simulation.
    Why does it rotate the coordinates?
    It's supposed to be milling the face of the tapered cylinder (cue).
    You are using Y twice, maybe causing a Z default. Are you using G17/18/19 to set plane ?

    A rotary axis is usually labelled A,B or C (by convention) so I've never seen one labelled Y before.

  3. #3
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    Im not sure if you are familiar with how to design for fourth axis? You cannot create a four axis coordinate system, the 4th axis is defined in mill settings... or am I missing something?

  4. #4
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    What Solidworks version you use?
    I can't see any attached thumbnails on your first post.
    Share your file and I can check what is wrong.
    Edit:
    Quote Originally Posted by viroy View Post
    I am running a 4-axis tree mill... chinese wood mill system, 2.2kw 3-axis with rotary A-axis.
    Also A axis is along X.
    B axis is along Y.
    Those are standard.

    Quote Originally Posted by viroy View Post
    Im not sure if you are familiar with how to design for fourth axis? You cannot create a four axis coordinate system, the 4th axis is defined in mill settings... or am I missing something?
    You need to create a coordinate system for your part for CAM to know your part orientation in relation to that coordinate system.

  5. #5
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    The software on the workstation is Solidworks 2022 Premium which looks to be bundled with 'Solidworks CAM' that comes with it.

    The machine working area is 2ft X-axis travel by 4ft Y-axis travel.
    The rotary A-axis is 3ft long and only fits on the longer Y-axis.
    So I create a coordinate system with the Y-axis running down the length of the cue, Z-axis is up.

    Then I setup the rotary by selecting 'define machine', then go to the 'rotary axis' tab and where it says "rotary axis is..", I select 'Y-axis' and set "0-degree position" to 'XY Plane'.
    When I 'extract machinable features' and simulate, it changes the Y-axis coordinate to Z-axis and wants to mill just the ends from the Z-axis.

    If I change 'rotary axis is..' to the 'X-axis' and 'extract machinable features', im guessing it finds nothing because it wont allow 'generate operation plan' to make toolpaths.

    Click image for larger version. 

Name:	Correct Axis.jpg 
Views:	2 
Size:	65.5 KB 
ID:	489789
    Click image for larger version. 

Name:	Wrong Axis.jpg 
Views:	1 
Size:	43.6 KB 
ID:	489791
    Here you can see how in design it shows the Y-axis running along the cue length.... but when I create a toolpath and simulate, the Z-axis now runs down the cue length instead and mills on the ends of the cue rather than the face.
    Last edited by viroy; 02-25-2023 at 04:39 PM.

  6. #6
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    Again attachment not showing for me.
    If your rotary axis is along Y axis, you need to name it B axis, not A axis.
    In camworks NC manager window you need to define:
    1. Machine
    2. Stock
    3. Coordinate System (selecting your made one, or other options)
    4. Create Setup (where you select the plane perpendicular to Z and watch for direction, can be changed)
    Only after that you can extract machinable features, but those are only for known features in solidworks like pokets, holes and others.
    You can attach here your solidworks part file if you want me to look at.

    Edit:
    To resolve your B axis in CAM you need to open Technology Database and go to Mill select Mill 4 axis mm or inch and click COPY.
    Name it as you wish in right panel and go down to last tab Setup where you select rotary axis as Y, then Save.
    Now select that machine that you just made.
    You also need to make a post processor for it to generate usable g-code, predefined one are only for demonstration propose.

  7. #7
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    Oh I think I see why, the size limit is 97kb for images... ill resize
    I cannot upload the solidworks file... this site limits to 100kb and the file is 270kb
    Attached Thumbnails Attached Thumbnails Correct Axis.jpg   Wrong Axis.jpg  
    Last edited by viroy; 02-25-2023 at 06:44 PM.

  8. #8
    Join Date
    Apr 2018
    Posts
    130

    Re: Axis orientation flips

    I too saw no images in this thread at CNCZone. But I retrieved these images from CNCZone's sister forum site, Industry Area, and they are posted below:

    Attachment 489794
    Attachment 489792

    I don't have a good explanation of how this occurs, but I don't think this is something caused by the way the files were posted.

  9. #9
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    Click image for larger version. 

Name:	Correct Axis Small.jpg 
Views:	1 
Size:	58.1 KB 
ID:	489799
    Click image for larger version. 

Name:	Wrong Axis Small.jpg 
Views:	1 
Size:	47.3 KB 
ID:	489801
    Can you see them now?

  10. #10
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    The opertations I need to perform are face milling the cue from a uniform cylinder to a tapered cylinder... then cut the pockets. Thank you so much for helping!

  11. #11
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    Thank you RaderSidetrack.
    Viroy I have sent you a private message.

  12. #12
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    Quote Originally Posted by viroy View Post
    Oh I think I see why, the size limit is 97kb for images... ill resize
    I cannot upload the solidworks file... this site limits to 100kb and the file is 270kb
    I had attached larger file like this
    File-size
    296.9 KB
    Downloads
    2
    Date Posted
    02-07-2023, 05:06 PM
    without any problem.

  13. #13
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    Now I see what is wrong.
    https://www.solidworks.com/product/solidworks-cam
    3 + 2 Programming
    SOLIDWORKS CAM Professional can employ a machining technique where a three-axis milling program is executed with the cutting tool locked in a tilted position using the five-axis machine's two rotational axes.


    You can not make 4 axis simultaneous machining. Only 3 + 2, but that 3 axis simultaneous is only for linear axis, not 2 linear and 1 rotary = 3 axis.
    I was confused because I use camworks in solidworks witch is 5 axis simultaneous capable.

    So you can make 3 axis toolpaths from diffrent positions around your part, but your rotary axis is only for positioning in Solidworks CAM.

    Something like this:
    Click image for larger version. 

Name:	example.jpg 
Views:	2 
Size:	52.0 KB 
ID:	489816

  14. #14
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    So then I cannot cut the pocket in my design with this version?
    I did figure out how to index the A axis and then make a 3 axis cut, but I cannot get it to roll the A-axis while cutting.
    I own my own machine but am using workstations at a tech school to design (sworks too much $ to buy)... there are older versions available for me to use. What would you recommend?

  15. #15
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    Solidworks does not help you, any version, without a CAM package for Solidworks, but those are expensive too.
    There is a freecad with CAM, but I don't have experience with and don't know if it support full 4 axis (I think is a wrap function for rotary).
    Also from what I read popular Fusion 360 is expensive too for more then 3 axis.
    There are more like Deskproto, Vectric Aspire and so on. You need to check them to see what fits your need, also your budget.

    Edit:
    And there is a hard way to make toolpaths for free manually. For your part is not very complicated, but you can do that if you need to program once and make many parts.
    Example:
    For conical part if larger diameter is on 0 position and have 30mm, smaller diameter is 20mm and length 1000 mm will be like this
    G0 X0Y0
    G0 Z20
    G1 Z15 F500
    G1 Y1000 Z10 B180000 F1000
    G0 Z20
    G0 X0Y0
    Don't use this without a header, it is just an example.

  16. #16
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    There is a station I can use which has CAMworks 2020... I've never used camworks, hope its similar.
    Also theres a station with Solidworks 2011 & SolidCAM 2010

  17. #17
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    Solidworks CAM is made by HCL witch made CamWorks, so is the same but better, you can do 4 or 5 axis simultaneous machining.
    You only need a post processor for your machine, if you have problems with that, I can help you.

  18. #18
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    Thanks, I'll get started on one of them hopefully today.
    I'd like to prepare for needing a post processor just to get that out of the way.
    When I was doing 3-axis programming, I used the built in Fanuc PP.
    The only one I have is a mori-seiki 4-axis, no idea if it will work or not... I'll attach it here
    Attached Files Attached Files

  19. #19
    Join Date
    Mar 2008
    Posts
    452

    Re: Axis orientation flips

    ok so I have to use Solidworks 2011 with solidcam 2010.

    ------------------- Mill Results ---------------------------
    I have tried using just 'Mill' create paths, but the '4-axis' option is greyed out and will only do 3-axis cuts.

    ------------------- Mill-Turn Results ----------------------
    I have gotten a simultaneous 4-axis cut to successfully simulate by using 'mill-turn' instead of 'mill'.
    Unfortunately I cannot simulate using 'SolidVerify', its greyed out... only options are 'Host CAD' and '2D'.
    Sim with host cad shows it rotating while cutting and is following the pocket, looks like a good result!

    but, when I look at the output... the rotary axis is C-axis rather than A-axis... I use Mach3 on my CNC and I saw you can define both C-axis and A-axis, so I'm assuming it doesnt really matter if the g-code output is for A or C.

    The only post processor solidcam mill-turn has is 'Nakamora'.
    When I try to produce G-code it gives an error:
    "Warning: This is not a production ready post and must be modified to the machine tool requirements before use"
    The G-code output looks very wicked, nothing like I normally see.... and I only see C, X and Z axis instructions, there should be lots of Y-axis as that runs the length of the stock... I would guess 90% of the code is C-axis

    Is this caused by not having the right post processor?

  20. #20
    Join Date
    Aug 2011
    Posts
    252

    Re: Axis orientation flips

    Quote Originally Posted by viroy View Post
    I use Mach3 on my CNC and I saw you can define both C-axis and A-axis, so I'm assuming it doesnt really matter if the g-code output is for A or C.
    In fact that matters the most.
    As I said before you can not run A axis along Y, and swapping axis names will only confuse you.
    A axis is rotary along X axis, B axis is rotary along Y axis and C axis is rotary along Z axis.
    You need to start from this.

Page 1 of 6 123

Posting Permissions

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