584,866 active members*
5,090 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Visual Mill > stl's or iges or dxf's for 3axis milling?
Results 1 to 20 of 20
  1. #1
    Join Date
    May 2006
    Posts
    89

    stl's or iges or dxf's for 3axis milling?

    Which file format is the best most complete and user freindly for 3 axis and 2.5 D machining with VM5 ? I am using Alibre for 3D modeling and exporting in either format. Which is best and easiest to work with as far as selecting regions, curves, surfaces etc.? Also depending what file is best, how should the file export details be set in Alibre to best suit VM 5?
    Exotic Welder

  2. #2
    Join Date
    Jan 2006
    Posts
    4396
    When recieving files from Alibre I request STEP files. This is by far the best file extention translator in my opinion. IGES being the worst. Recieved a few Iges and had to reposition all 3 axies from about 300 inches or so. DXF is usually used for 2D wireframe not Solid Models. As for STL extentions I've never used them.

    Honestly you should try them all to see which one you like best. Most of this stuff is all trial and error.

    :cheers:
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

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

    www.refractotech.com

  3. #3
    Join Date
    May 2006
    Posts
    89

    What Cam program?

    What CAM program do you use, I dont think VM5 can open STEP files.
    Exotic Welder

  4. #4
    Join Date
    Jan 2006
    Posts
    4396
    Quote Originally Posted by dave6
    What CAM program do you use, I dont think VM5 can open STEP files.

    BobCAD-CAM, and I believe you will have to purchase a STEP File Translator from Mecsoft.
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

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

    www.refractotech.com

  5. #5
    Join Date
    Oct 2006
    Posts
    6
    Iges files work fine in VM5. It is essentially the same thing as step, an arrangement of mathmaticaly interpolated sufaces that are smooth at any resolution. These are called NURBS surfaces (Non-rational Uniform B-Splines) What you need to know is this. Stl's and DXFs are polygon surfaces. This means the surface is made up of tiny squares or triangles. The resolution is fixed, and can only be increased by complex algorithms found in expensive poly modeling packages like MAYA or 3D Max. Even then, the polygon layout must be clean and ordered. You also need to know that VM5 reduces Iges, STEP and other math models down to polygons when you import them based on tolerences you set in machining options. This can confuse the he!! out of beginners, because VM has low default tolerance settings, resulting in jagged cuts on an object that should be smooth. For anything with small features, like curves with a radius under 1", reset your import tolerances to at least 0.001". try 0.0005", if you have a decent computer. Most cad software lets you set all these tolerences in the export dialoge for STL's or DXF's, so it almost doesn't matter where you do it, before VM5 or in VM5, but dense STL's are huge hard drive lumps. I will say I have found better controle of how a surface is reduced to poly in Rhino 3 than in VM5 or any other package. One last reason to bring Iges files into VM. Curves and regions seem to be extracted best when VM does the poly reduction its self.
    Hope this all helps

  6. #6
    Join Date
    May 2006
    Posts
    89

    Smile Thanks

    Thanks for the reply I will look into these settings further.
    Exotic Welder

  7. #7
    Join Date
    Mar 2003
    Posts
    63
    Since Alibre is ACIS based. Is the native ACIS extension .sat, .stp or other?

  8. #8
    Join Date
    Mar 2008
    Posts
    3

    Unhappy Help me out Guys

    Hey Friends
    The VM 6.0 gives me an error whenever i try to open a cad design of about 97MB
    It says " Out of Dynamic Memory "
    What shouls i DO?????
    Please anyone help me out

  9. #9
    Join Date
    Jan 2004
    Posts
    3154
    Have you tried [email protected]
    www.integratedmechanical.ca

  10. #10
    Join Date
    Mar 2008
    Posts
    3

    Smile Ya i tried

    Hello sir
    I hv send my prob to them but not yet recieved any reply from them
    could u suggest any other software for 4axis roatry toolpath generation

  11. #11
    Join Date
    Jan 2004
    Posts
    3154
    They dont work on weekends.
    Usually they make their responses by noon Pacific Time USA - which is likely around midnight your time?
    I notice you posted on the forum, did you also send the email?
    You are not guaranteed a response on the forum (although you usually get one) but they always answer emails.
    www.integratedmechanical.ca

  12. #12
    Join Date
    Mar 2008
    Posts
    3

    Smile Thanks

    Hello,

    Thanks for helping me and i got an reply form mecsoft n they hv told some setings to try for getting the results.

    I am sorry for troubling you and taking your time for me. hope u dnt mind it

    Neways thanks again.

  13. #13
    Join Date
    Jun 2008
    Posts
    226
    Quote Originally Posted by Clever Monkey View Post
    You also need to know that VM5 reduces Iges, STEP and other math models down to polygons when you import them based on tolerences you set in machining options. This can confuse the he!! out of beginners, because VM has low default tolerance settings, resulting in jagged cuts on an object that should be smooth. For anything with small features, like curves with a radius under 1", reset your import tolerances to at least 0.001". try 0.0005", if you have a decent computer. Most cad software lets you set all these tolerences in the export dialoge for STL's or DXF's, so it almost doesn't matter where you do it, before VM5 or in VM5, but dense STL's are huge hard drive lumps. I will say I have found better controle of how a surface is reduced to poly in Rhino 3 than in VM5 or any other package. One last reason to bring Iges files into VM. Curves and regions seem to be extracted best when VM does the poly reduction its self.
    Hope this all helps
    OK,

    How does VM6 reduce models to polygons? Which is the golden rule here?

    1. Create the model in SW, save as iges. Yes/No??
    2. Start VM6, set import tolerances to 0,01mm and import the iges file.Yes/No??
    3. Where does Rhino3D come in if you say that VM is still better anyway?

    If I use VM6 with mm settings, to what values do I set:

    Part Faceting Tolerance?

    Curve Hookup Tolerance?

  14. #14
    Join Date
    Jan 2004
    Posts
    3154
    Quote Originally Posted by CNC Viking View Post
    OK,

    How does VM6 reduce models to polygons? Which is the golden rule here?

    1. Create the model in SW, save as iges. Yes/No??
    2. Start VM6, set import tolerances to 0,01mm and import the iges file.Yes/No??
    3. Where does Rhino3D come in if you say that VM is still better anyway?

    If I use VM6 with mm settings, to what values do I set:

    Part Faceting Tolerance?

    Curve Hookup Tolerance?

    1) Yes (recommended export settings are in the pic). VM also has an SW import module that integrates with SW and removes the need for extra translations - I really like it.

    2) .01 mm should be good (IMO really fussy would be .003mm) the finer settings can really choke a good computer - fast. There is NO golden rule, every project depends on what finish, tolerance, MOP, and physical size is used/required. Faceting ONLY effects 3D based MOPS AND a lot of the MOPS have "Fit Curve" functions that will remove the Polys altogether. The ones that don't have this function, you can do in the toolpath editor (Pro version).

    3) Rhino is CAD and VM is CAM, not sure what you mean? Some people believe that Rhino makes for the best "middle-man" translator, but I have not had any issues with any file that is on VM's import list.

    4) Typically I set Curve hook-up to .05mm My only reason is for some poor quality DXF conversions that can sometimes come through without lines joined.

    5) Typically I do everything I can with 2.5D milling (off of a DWG/DXF that I create in SW). It may seem counter-tech and non-intuitive but, for the extra 2 minutes it takes to make a "proper for CAM" DWG I usually save well over 1/2 hour in programming and computing time (some 3 axis toolpaths can easily take 1/2 hour each to generate, especially if you haven't figured out the tricks/settings to keep the compute time down).
    K.I.S.S. applies heavily.
    Attached Thumbnails Attached Thumbnails IGS out.jpg  
    www.integratedmechanical.ca

  15. #15
    Join Date
    Jun 2008
    Posts
    226
    DareBee,

    Thanks for the nice answer.

    It really helps as I am pretty much on square #1 on CAM learning curve at the moment.
    Have pretty much set my mind on VM6 Pro though.


    1. So which is best then .sldprt or iges? And is the .sldprt translator fully included in VM6 or just an optional add-on to pay licence for each year? If one choses to export .sldprt files, are there settings to tweek as well before sending it off to VM6? I do not have SW now, but it is the CAD i have easiest access to by borrowing friends' seat.

    2. OK, now I at least know the ballpark.

    3. I mean, is there any reason to first export a .sldprt file to Rhino3D and then to VM6? And what shall I do with the file in Rhino3D?

    By the way, is Rhino's .3dm fileformat any good? Is there anything to gain by translating .sldprt to .3dm and then sending it to VM6?

    4. So curve Hookup "mends" broken lines? I always thought that you MUST find those and repair by correcting it in the CAD, before proceeding to CAM?

    5. Yes, I agree, at least if you have vertical valls and chamfers. When I come to true 3D machining I will howl again.

    And you know what? I am in the progress to add a true continious 4:th axis to my VMC.

  16. #16
    Join Date
    Jan 2004
    Posts
    3154
    Quote Originally Posted by CNC Viking View Post
    DareBee,

    1. So which is best then .sldprt or iges? And is the .sldprt translator fully included in VM6 or just an optional add-on to pay licence for each year? If one choses to export .sldprt files, are there settings to tweek as well before sending it off to VM6? I do not have SW now, but it is the CAD i have easiest access to by borrowing friends' seat.

    2. OK, now I at least know the ballpark.

    3. I mean, is there any reason to first export a .sldprt file to Rhino3D and then to VM6? And what shall I do with the file in Rhino3D?

    By the way, is Rhino's .3dm fileformat any good? Is there anything to gain by translating .sldprt to .3dm and then sending it to VM6?

    4. So curve Hookup "mends" broken lines? I always thought that you MUST find those and repair by correcting it in the CAD, before proceeding to CAM?

    5. Yes, I agree, at least if you have vertical valls and chamfers. When I come to true 3D machining I will howl again.

    And you know what? I am in the progress to add a true continious 4:th axis to my VMC.
    1) SLDPRT. I have not had trouble with translations but theory says that things CAN be lost in translation (you ever worked with prints translated from German or worse - Japanese? yeesh) Translator is NOT included and is listed as $500 on the website. AFAIK it is a oneshot price (but it is possible that an upgrade cost may incur for new versions of VM as they are released)

    3) IDK - I just hear some people going on about it. IMO why would you spend good money on a program to use for translating when you can buy the SW plug-in?

    4) See - I just saved you some time.

    I do 3+1 and 4 axis work as well.

    BTW there is a forum at MecSoft.com and support or sales are very nice there. They will answer any questions you ask and do over the net demos for you on your own supplied parts.
    www.integratedmechanical.ca

  17. #17
    Join Date
    Sep 2004
    Posts
    107
    Quote Originally Posted by CNC Viking View Post
    3. I mean, is there any reason to first export a .sldprt file to Rhino3D and then to VM6? And what shall I do with the file in Rhino3D?

    By the way, is Rhino's .3dm fileformat any good? Is there anything to gain by translating .sldprt to .3dm and then sending it to VM6?
    If you've got a seat of Rhino you can pay a bit extra to MecSoft and get the dongle set so you can run VM inside of Rhino as RhinoCAM. I haven't done any projects in RhinoCAM yet, but I just now tried opening one of my Rhino files and went through the first steps in RhinoCAM as I would in VM6 (stock box, set WCS) and then I picked a 3D region for horizontal roughing and, well, it just picked it. There was no visible conversion to something that VM might like better.

    So if you've got Rhino and are familiar with it RhinoCAM might save you some conversion bother.

    I'll note that VM seems to like a 2D DXF out of Rhino better than it does one from Alibre. The Rhino features seem to be more likely to be one solid curve instead of a bunch of small segments that have to be joined together.

    I know one programmer/machinist who really likes working in RhinoCAM. It sounds like part of that is due to the many surfacing commands available in Rhino, and that he doesn't have to move in and out of CAM to CAD to CAM if he wants to tweak something.

    Your mileage may vary on that as I'm just getting somewhat comfortable with not terribly complicated 2.5D work, and I haven't done any 3D stuff yet.

    cheers,
    Michael

  18. #18
    Join Date
    Sep 2004
    Posts
    264
    Just a couple of added notes as far as faceting tolerances etc. in VM and RhinoCAM.

    In VM, when you import the part, it meshes the entire model with your faceting tolerances, as VM doesn't understand anything but meshes. All your volumes/surfaces are converted to mesh and that faceting tolerance is then fixed. So if you want fine finishing toolpaths, you need to have fine faceting import tolerances, and that will make your model very heavy.

    In RhinoCAM you have the advantage that the parts remain in NURBS format all the time. The toolpaths are calculated on instantaneous meshes created at the time of launching the toolpath calculation and are based on the tolerances you set in the operation. Thus, if you have a roughing toolpath, you don't need to have a fine mesh. The advantage is that you can set the finishing paths as fine as you want without having to worry about whether you faceted your part fine enough... you don't have to worry about faceting at all.

    Rhino's drawing and part creation tools are also far superior to those in VM - that's to be expected, Rhino is a full fledged 3D CAD program - and it is outstanding as a tool for fixing other CAD models and preparation for machining. Even if you are only going to use Rhino as an editor in that sense, I think the ease of use is well worth the extra money to buy a seat of Rhino with RhinoCAM instead of VM. But that's just my opinion...

    --ch

  19. #19
    Join Date
    Jun 2008
    Posts
    226
    chmillman,

    Now, that was VERY interesting to read.:cheers: I have been thinking of RhinoCAM2 as well. Is RhinoCam2 only available as a package with Rhino4 CAD? MecSofts website says that Rhino4 have to be installed prior to installing RhinoCam2. Has RhinoCam2 got the SW (.sldprt) translator plug-in as standard?

    So let's say I import an .sldprt file from SW into RhinoCam2.

    What is needed to be done at the SW side and/or the RhinoCam2 side? Where are those tolerance levels decided/set?

    What fileformat will it get when imported into RhinoCam2?

    About Rhino4 CAD: I have heard/read that it is not parametric and only have data of the surface and thus is no real alternative to SW? Tru or false?

    Please explain this in a simple to understand way.

  20. #20
    Join Date
    Sep 2004
    Posts
    264
    1) RhinoCAM (2.0) is simply Visual Mill 6 that runs inside Rhino as a plug-in. Rhino is the CAD framework for the CAM part which is plugged-in. RhinoCAM cannot run on its own, if you need a stand-alone package, you buy VM 6.

    2) The translators of different file formats are thus Rhino's translators, not Visual Mill's. Rhino imports and exports a far greater variety of formats than does Visual Mill, including a sldprt importer (which is also FREE - no sldprt export, though).

    3) File tolerances are set in Rhino for the geometry. You can set them any way you want. For toolpathing, they are set in the individual operations when you specify your machining tolerances. I do not know what needs to be done inside Solidworks - if anything - before the file is ready for CAM. I do import Solidworks files regularly, and they're usually perfect.

    4)When files are imported into Rhino they are translated into the native Rhino format (.3dm). They can be exported in a wide variety of other formats.

    5) Correct, Rhino is not parametric. You have curve, surface, volume and mesh data, but none of it is parametric. As far as being "no real alternative to SW" that is a matter of needs, personal opinion, philosophy and working methods. Parametrics are not necessarily obligatory for many things. It depends on what you need to do.

    You can also add SpaceClaim to Rhino do be able to do direct "solid" editing.

    HTH, --ch

Posting Permissions

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