oneCNC datum setting
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Feb 2018
    Country
    UNITED KINGDOM
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Post oneCNC datum setting

    I've recived a STEP file from a coustomer , when I open it in one cnc the cad veiw is the side face . When I move my datum it only alters X,Y . How do I rotate the job/face reffrence so the part is relevent the the machine. I am trying to do this so i can load the part into mastercam mill version 8.1.1

  2. #2
    Join Date
    Oct 2004
    Location
    Elyria Ohio
    Posts
    1,647
    Post Thanks / Like
    Likes (Given)
    2895
    Likes (Received)
    597

    Default

    Quote Originally Posted by [email protected] View Post
    I've recived a STEP file from a coustomer , when I open it in one cnc the cad veiw is the side face . When I move my datum it only alters X,Y . How do I rotate the job/face reffrence so the part is relevent the the machine. I am trying to do this so i can load the part into mastercam mill version 8.1.1
    Hi Connor - Just highlight your model and then perform a "rotate" function to position the part the way you want to machine it. That's how I handle it.

    So if it takes me two or three positions (or 4 or 5) I will rotate the part and call it "first op" then "second op" and so on. And I will save that file with that name so that I can refer back to it if I have to make more than one of something. If you're running a 4 or 5 axis machine then it will be even easier because you will probably be able to machine just about any part in two setups.

    I have never been overly successful in trying to shift the datum around so I move the part around the datum and have found it to be much easier and I get a better result.

    If you have a question you can send me the file and I will rotate the part for you and send it back - then it will be easier for me to explain how I did what I did for you. Shoot me a pm and I will send you my email. You're in England so your a few hours ahead of us so if you are still at work send it to me soon because I am leaving at noon today and not working tomorrow. Joe
    Last edited by Joe Miranda; 02-23-2018 at 05:23 AM. Reason: addition

  3. Likes eaglemike, [email protected] liked this post
  4. #3
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Quote Originally Posted by [email protected] View Post
    I've recived a STEP file from a coustomer , when I open it in one cnc the cad veiw is the side face . When I move my datum it only alters X,Y . How do I rotate the job/face reffrence so the part is relevent the the machine. I am trying to do this so i can load the part into mastercam mill version 8.1.1
    If you are using Onecnc xr5 there is a function called in car position, or move to/from plane. It's not easy to explain on the internet, but watch some youtube videos. It's way easier and faster than trying to rotate and translate.

  5. Likes HuFlungDung liked this post
  6. #4
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Rotating the part in different files is crazy. Your simulation wont work. I don't know what software you are using, but you should be able use more than one WCS in a file.

  7. #5
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,609
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    3293

    Default

    Quote Originally Posted by TRussell View Post
    Rotating the part in different files is crazy. Your simulation wont work. I don't know what software you are using, but you should be able use more than one WCS in a file.
    Yes, OneCNC has "3 axis repositioned" as one of the cam functions for machining multisided parts without actually rotating the model in 3d space. Set it up initially with "In car position" and then leave it there and machine all sides, selecting "3 axis repositioned" before selecting a new plane position to begin creating machining ops thereon.

  8. #6
    Join Date
    Oct 2004
    Location
    Elyria Ohio
    Posts
    1,647
    Post Thanks / Like
    Likes (Given)
    2895
    Likes (Received)
    597

    Default

    Quote Originally Posted by TRussell View Post
    Rotating the part in different files is crazy. Your simulation wont work. I don't know what software you are using, but you should be able use more than one WCS in a file.
    I will look for the youtube vid on this and see if I can make sense out of it. But to say that rotating the files is crazy and that the simulation won't work - that's crazy - of course it works - I use it all the time - why wouldn't it work? You can rotate the piece wherever you want it in space and still use simulation.

  9. #7
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Quote Originally Posted by Joe Miranda View Post
    I will look for the youtube vid on this and see if I can make sense out of it. But to say that rotating the files is crazy and that the simulation won't work - that's crazy - of course it works - I use it all the time - why wouldn't it work? You can rotate the piece wherever you want it in space and still use simulation.
    If you are using more than one operation, your simulation will not be accurate for both. Moving the part in CAD, instead of moving the WCS is the wrong way to do it. If you have a part with two operations, you can set up your first WCS wherever you want it using planes, without translating the model. Then move your WCS to the other side, now you can simulate the entire program, including the move. If you move the part, you are stuck simulating one operation at a time. Trust me, figure this out, and you will wonder how you did things before.

  10. #8
    Join Date
    Jun 2006
    Location
    Finland
    Posts
    421
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    49

    Default

    Onecnc (at least XR5) doesn’t support moving your WCS. You have to orient the part and use the repositioning for other sides. Brainless and annoying, but that’s how it is

  11. #9
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Quote Originally Posted by Harri View Post
    Onecnc (at least XR5) doesn’t support moving your WCS. You have to orient the part and use the repositioning for other sides. Brainless and annoying, but that’s how it is
    I'm using XR5, and I do it all the time, I think it depends on what level you bought. I think I'm using pro.

  12. #10
    Join Date
    Jun 2006
    Location
    Finland
    Posts
    421
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    49

    Default

    I also used Pro. I still think there is no way of moving the WCS, only the part. And this means you have to re-pick paths. Correct me if i'm wrong and you'll spoil my days for the past 10 years

    I know there is offset under posting or somewhere, but you still can't rotate, flip or move the actual WCS.

  13. #11
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Quote Originally Posted by Harri View Post
    I also used Pro. I still think there is no way of moving the WCS, only the part. And this means you have to re-pick paths. Correct me if i'm wrong and you'll spoil my days for the past 10 years

    I know there is offset under posting or somewhere, but you still can't rotate, flip or move the actual WCS.
    At the upper right hand corner of your Cam manager there should be an icon you can click on to bring up a menu that includes 3 axis, 3 axis repositioned 4 axis position, 4 axis simultaneous, 5 axis position, and 5 axis simultaneous. Use 3 axis reposition and set up a plane using 3 points, this is now the origin of your new WCS.

  14. #12
    Join Date
    Jun 2006
    Location
    Finland
    Posts
    421
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    49

    Default

    Yes, _before_ you create a toolpath. Once it's created you can't move the WCS origin as far as I know.

  15. #13
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Quote Originally Posted by Harri View Post
    Yes, _before_ you create a toolpath. Once it's created you can't move the WCS origin as far as I know.
    Yeah, you have to pick your WCS before you generate a toolpath. How would you do it after? Are we talking about the same thing here? I'm talking about choosing the plane and origin, before you generate a toolpath, then moving the origin without translating the part to generate another toolpath on another face. You have to do this, so you can simulate more than one setup.

  16. #14
    Join Date
    Jun 2006
    Location
    Finland
    Posts
    421
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    49

    Default

    I meant the possibility to move or rotate a wcs after toolpath generation, Z axis direction remaining the same. Most CAM packages have this feature, just grab the wcs origin and place it where you like.

  17. #15
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Quote Originally Posted by Harri View Post
    I meant the possibility to move or rotate a wcs after toolpath generation, Z axis direction remaining the same. Most CAM packages have this feature, just grab the wcs origin and place it where you like.
    I think you can move the origin of some toolpaths by using the repeat operation function, and turning off the original. You can also switch planes.

  18. #16
    Join Date
    Jun 2006
    Location
    Finland
    Posts
    421
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    49

    Default

    Workarounds do help, but IMO it would be much nicer to have the possibility to freely move and rotate the WCS (as long as Z direction is maintained).

    Onecnc does a lot of 2.5D stuff really well, but it does have some very annoying limitations. You get what you pay for.
    Before the appearance of Fusion360 it was probably the best money to value alternative in low-budget CAM.

  19. #17
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    9,609
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    3293

    Default

    OneCNC allows you to drag and drop an operation from one toolpath group into any other toolpath group. It will maintain the WCS for that operation, it does not 'fix it' automatically. There is some power in that, some functionality that goes beyond automatic updating of operations, IMO. You can also record all parameters of an operation in a template, then fix the WCS and generate a new operation in a few clicks. Not that difficult.

    There are trade-offs to be made, no matter what flavor of CadCam you want to use. At some point, you'll most likely get in a bind doing some sort of 'impossible' scenario that either wasn't anticipated, or was deliberately avoided due to the far reaching consequences of making a 'small change'.

    OneCNC does 3d stuff really well, too. In fact, 3d machining is pretty much automated: put the model on screen and toolpath it. It doesn't go ahead on its own and update all the ops until you pull the trigger, but again, that has its advantages, as you can drag operations across groups and still have it do exactly what it did in another operation. You're not 'stuck', you can update it to the model if you wish. But maybe it doesn't need updating, so no processing time wasted.

    I love getting a mold cavity machining job: relaxation time!

  20. #18
    Join Date
    Jun 2006
    Location
    Finland
    Posts
    421
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    49

    Default

    I left Onecnc around XR5, so I can’t comment on the newer versions, but I humbly beg to differ regarding 3D work. I probably knew almost all the possible tricks and then a few, but still feared complex 3D work. Some of our work just got too complicated, whatever you did. But these are just opinions, you have yours and I have mine

  21. #19
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    Quote Originally Posted by HuFlungDung View Post
    OneCNC allows you to drag and drop an operation from one toolpath group into any other toolpath group. It will maintain the WCS for that operation, it does not 'fix it' automatically. There is some power in that, some functionality that goes beyond automatic updating of operations, IMO. You can also record all parameters of an operation in a template, then fix the WCS and generate a new operation in a few clicks. Not that difficult.

    There are trade-offs to be made, no matter what flavor of CadCam you want to use. At some point, you'll most likely get in a bind doing some sort of 'impossible' scenario that either wasn't anticipated, or was deliberately avoided due to the far reaching consequences of making a 'small change'.

    OneCNC does 3d stuff really well, too. In fact, 3d machining is pretty much automated: put the model on screen and toolpath it. It doesn't go ahead on its own and update all the ops until you pull the trigger, but again, that has its advantages, as you can drag operations across groups and still have it do exactly what it did in another operation. You're not 'stuck', you can update it to the model if you wish. But maybe it doesn't need updating, so no processing time wasted.

    I love getting a mold cavity machining job: relaxation time!
    I agree that OneCNC is easy to use for 3d, but then again, so is most modern CAM software. My problem with OneCNC is with 5 axis simultaneous. It's easy and fast to get a toolpath, but if you don't like what you get, you're screwed.

  22. #20
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    80
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    25

    Default

    I forgot to add that the reason I chose OneCNC was that the 5 axis positional was so easy to use. That part works better than anything else I looked at 5 years ago.


Tags for this Thread

Bookmarks

Posting Permissions

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