Importing rhino hull to solidworks?

Discussion in 'Software' started by sea state, Nov 12, 2009.

  1. sea state
    Joined: Nov 2009
    Posts: 8
    Likes: 0, Points: 0, Legacy Rep: 10
    Location: USA

    sea state Junior Member

    I am having some trouble importing my hull shape from Rhino into solidworks. I can get an IGS hull into solidworks, but there are gap problems at the edges. It won't allow me to thicken the surface to make a hull part. The hull is generated from Rhinomarine, basically I just started with the default planing hull from the wizard to get the process down. If you zoom way in, you can see some irregularities.

    Does anybody have this process down? Any lessons learned you can share? Are some file formats (IGS, step, parasolid) better than others? What is the best way to make a hull part, thicken the surface, or use the surface as a mold and extrude to it, then shell it?

    Any insight?
     
  2. ruysg
    Joined: Feb 2008
    Posts: 36
    Likes: 1, Points: 8, Legacy Rep: 10
    Location: Sao Paulo, Brazil

    ruysg Junior Member

  3. sea state
    Joined: Nov 2009
    Posts: 8
    Likes: 0, Points: 0, Legacy Rep: 10
    Location: USA

    sea state Junior Member

    what does plug-in do that SW doesn't?

    Solidworks is supposed to open rhino files directly. I'm not sure what the plug-in does that SW isn't supposed to be able to do. However, when I generate a hull in rhinomarine, and save as a rhino file, it won't open in SW. Says there are no surfaces or solidworks. When I save the same hull as IGS, it comes in fine, but is still troublesome to work with.
     
  4. Michael Chudy
    Joined: Apr 2005
    Posts: 39
    Likes: 1, Points: 0, Legacy Rep: 16
    Location: Eastport, Maine

    Michael Chudy Yacht Designer

    I'm sure you paid a good price for Solidworks. Doesn't that come with customer support? Have you asked them?
    Mike
     
  5. dougfrolich
    Joined: Nov 2002
    Posts: 661
    Likes: 21, Points: 28, Legacy Rep: 225
    Location: San Francisco

    dougfrolich Senior Member

    Sea state-
    Make sure you have a valid surface in Rhino first.
    if yes, and it still will not thicken--try importing only the 1/2 hull.
    if you have multible surfaces try them one at a time.
    If you still have trouble post an example of the problem.
     
  6. alidesigner
    Joined: Nov 2006
    Posts: 187
    Likes: 5, Points: 0, Legacy Rep: 93
    Location: Australia

    alidesigner Senior Member

    Try these.
    offset the surface with 0 offset then thicken the new surface (which is now solidworks native)
    or

    offset the surface by the thickness of the plate and then thicken the offset surface in the other direction, ie back towards the original hull surface.
     
  7. sea state
    Joined: Nov 2009
    Posts: 8
    Likes: 0, Points: 0, Legacy Rep: 10
    Location: USA

    sea state Junior Member

    Mike, I may go that route, but I was trying to leverage the experience here because a popular opinion seems to be rhino (marine or orca) to solidworks seems to be a great way to go for hull modeling. Surely someone has conqured this problem. So far I haven't figured out a decent way to make that work. I'm sure solidworks help will probably tell me I have a problem with my Rhino surface.

    Doug, I am not sure what you mean by make sure I have a "valid" surface in Rhino. At this point, I have opened Rhino, opened the hull wizard in Rhinomarine, hit OK to generate the hull (without changing ANYTHING). When I try to open as a Rhino file in solidworks, it says there is no surface or solid data. When I open as an IGS file, it comes in fine, but I am having trouble turning it into a proper hull shell. I have tried both the whole hull and half.

    Ali, I could offset the surface with 0 offset, but it still won't thicken. It won't offset more than 0.

    I have something wrong with the hull surface, but I am not sure what since I have changed nothing from the hull wizard. I think the problem is the intersection between the bottom and the topsides on the keel. Rhinomarine makes all these control points coincident, but the igs surface seems to be off a little bit. Not sure how to fix.

    I have tried the following:
    1. Thicken the imported surface.
    2. Offset 0 and thicken surface.
    3. extrude from a plane to the surface
    4. extrude from a plane to the offset
    5. offset hull thickness, and thicken back

    I have included the half hull in a couple different file formats if anyone wants to play with it.

    Thanks.
     

    Attached Files:

  8. dougfrolich
    Joined: Nov 2002
    Posts: 661
    Likes: 21, Points: 28, Legacy Rep: 225
    Location: San Francisco

    dougfrolich Senior Member

    I managed to thicken the imported surface. The chine flat has some mangled geometry in the original model near the bow which is what was not allowing SW to thicken. So I offset the surfaces to the inside deleated the chine flat, recreated it using the loft surface command then thickend the surface outward. I just picked .375" arbitrairly for the thickness.
     

    Attached Files:

  9. sea state
    Joined: Nov 2009
    Posts: 8
    Likes: 0, Points: 0, Legacy Rep: 10
    Location: USA

    sea state Junior Member

    Doug,
    Thanks for taking the time to fiddle with this. I was able to replicate what I think you did. However It seems the lines are not the same anymore, because the side of the hull offset mostly in, while the bottom offset mostly vertical. So when you loft between them, they form a different chine angle than the original geometry. And the final thickened version is not the same molded lines as the original. Part of the reason to start with Rhino marine is to rapidly see the hydrostatic properties as I adjust the hull lines.

    I thought I would fix it starting with offsetting the hull side and bottom with zero distance, loft the chine between the two, knit the surface, and thicken in. It won't let me thicken. I tried another method by bringing in the hull surface, mirror it, knit it together, then extrude from a plane, and shell it. It worked until the shelling part. Same story when I made a new chine and tried that method.

    I'm beginning to think I shouldn't start with the Rhinomarine hull wizard, although it gets me a rough shape to start from much quicker than the other methods within Rhino.

    I'm going to continue to experiment with it, and if anybody has suggestions or proven methods, I am certainly open to try them...
     
  10. dreamer
    Joined: Nov 2004
    Posts: 311
    Likes: 10, Points: 0, Legacy Rep: 188
    Location: Minnesota, USA

    dreamer Soñadora

    Sea state,

    I have done this hundreds of times (really). You should not have any issues importing from Rhino though knowing which version of each software you have would be most helpful. The Rhino (v.4) translator was available as a free add-on with SW-2008 (as long as you had maintenance) and is built-in to 2009. Previous versions will require you to use IGS (though I think the translator for Rhino actually came out with SP4 of 2007).

    As for thickening the hull, you do not want to use the 'thicken' command for precisely the reason you mentioned. You need to mirror the hull, close up the transom/stem then use either fill surface, loft, or boundary surface to fill in the deck. Boudary Surface will give you the best results. Make sure the whole thing knits up nicely then create a shell with your desired wall thickness.

    I will have a look at your models this evening.

    I haven't seen your model yet, but here's a pretty good rule of thumb:

    Chined hulls: model 100% in SolidWorks.
    Faired hulls: model the hull in something else (Rhinomarine or Orca - Orca is better, or even better: Maxsurf) and import into SolidWorks.

    Even better, if your surfaces are developable (i.e., curving in one direction only), use SolidWorks Sheetmetal and you'll be able to get accurate flat patterns.

    SWorks' surfacing tools are really great, but faired hulls are a real killer and it makes me sad that they cannot come up with better tools (such as a 'net' inference editor).
     
  11. foxy
    Joined: Aug 2009
    Posts: 25
    Likes: 1, Points: 0, Legacy Rep: 20
    Location: Florida

    foxy Junior Member

    Will try not to repeat other very good advice here.

    There are generally gaps in the models that I import from Rhino. Usually the simpler the model is, the easier it is to deal with. Try just importing the hull and add strakes or other features in SW. As mentioned, 32 bit SW has an import module for Rhino 3DM, however I usually have better luck with IGES. There is no import module for 64 bit SW so IGES is the only way to get the files in.

    Thicken does not work all that well when you have a radius of curvature that is small. You definitely don't want radii on a model you thicken. You generally want to extrude "up to surface" or extrude a box and trim with surface. In some cases, you can extrude something and then use the "replace face" command to get the shape. Its a matter of trial and error. After a while, you get a feel for what will work.

    After you get a solid, shell the part to the thickness you need. Shell may give you some warnings, but it will generally succeed and be usable. If shell doesn't work, its usually because of a very tight radius in the bow. Often you can do an extruded cut "offset from surface" which takes in most of the hull but avoids the area with the tight curvature.
     
  12. alidesigner
    Joined: Nov 2006
    Posts: 187
    Likes: 5, Points: 0, Legacy Rep: 93
    Location: Australia

    alidesigner Senior Member

    I downloaded your iges.

    The problem might be that you have modelled or exported it as 1 surface. It's easier if you have one surface for each plate, ie bottom, chine, sides.

    I dont use Solidworks anymore but I opened it and did all the offsetting etc in Inventor - no problems - but 1 surface at a time.

    Be carefull if you plan to flatten this in Solidworks. If you plan to use some tranverse curvature (which you should) then solidworks will flatten it as if it was a straight section and the internal structure wont fit. Compare the areas and section lengths of the flattened and unflattened parts.

    I also put it into maxsurf for a quick check, the bow area needs some work and it could use some transverse curvature but other than that it looks good. Rhino should be able to display some sort of Gaussian curvature plot to show this.
     
  13. dreamer
    Joined: Nov 2004
    Posts: 311
    Likes: 10, Points: 0, Legacy Rep: 188
    Location: Minnesota, USA

    dreamer Soñadora

    sea state

    After looking at this, I see that all you did was use the default starting powerboat model in Rhinomarine. I've worked with this model before. As ali pointed out, you'll want to make this into sections. All you really need to do is remove the chine. You can split that away from the rest of the model and either leave it in or delete it. I deleted it and simply used a loft to complete it once in SolidWorks.

    Then I mirrored the surfaces, extruded two surfaces for the transom and deck. I trimmed them all up, knitted to solid then shelled out to 3/8" thickness.

    Took all of 15 minutes. Most of that spent making screen captures.

    As for flattening, you will not be able to flatten anything from this model in SolidWorks. You have compound curvature and therefore undevelopable surfaces. You would need something like AeroHydro Surfaceworks to flatten. Really though, flattening for something like this is completely unnecessary if it's made from GRP.

    The nice thing about being able to import directly from Rhino vs. Iges is that it maintains associativity to the Rhino model. It's not an automatic associativity, but it simply takes a right click/update on the import feature to update. Very slick IMO.

    If you are using SW2009 or better, I'll be happy to give you the model.

    (note, images are not in order ;) )
     

    Attached Files:

  14. sea state
    Joined: Nov 2009
    Posts: 8
    Likes: 0, Points: 0, Legacy Rep: 10
    Location: USA

    sea state Junior Member

    thanks dreamer, ali, foxy

    dreamer,
    I am currently running Rhino 4 SR3 with RhinoMarine 4.0.3. For SW, I am running 2009 SP3.0.

    I was able to replicate your process until the point I tried to shell it. It gave me a crazy result. I then tried to add a fillet to the keel to see if that was a problem, and it wouldn't let me do that either. Is it best practice to do the detail surface work in Rhino, then import? Or better to get the basic shape in Rhino and add details in SW? I would love to have the part so I could see the exact process you used.

    Ali,
    yes, I just used the default geometry from the rhino marine hull wizard. I am not trying to build this hull, just trying to figure out the best process for going from Rhino to SW before I spend lots of time designing a hull and figure out I should have done it another way. I would like to start with the rhino marine hull wizard as a start because it gets me in the ballpark where I can adjust it easily. So I am not worried about fairness or flattening of this particular hull.

    Foxy,
    I would like to import using the 3dm file, but it says there is no surface or solid data when I try to open? Also, as I noted in my comments to dreamer, I had difficulty with the shell command. It came up with something, but it was a crazy shape. So I tried to add a radius to the keel line, but it won't let me do that (don't know why). I'll have to try the extruded cut with an offset surface.

    Thanks everyone for taking time to try to get me through this process.
     

  15. dreamer
    Joined: Nov 2004
    Posts: 311
    Likes: 10, Points: 0, Legacy Rep: 188
    Location: Minnesota, USA

    dreamer Soñadora

    sea state

    You will probably need to use a variable radius fillet. When you shelled, what thickness did you use?

    Shelling can be a bit dicey at times. A 0.25" thickness might not work, but a 0.251" might work. I used .375" and it worked fine. Adding fillets as you attempted will help. Usually the shelling is an issue in the stem which is where you are probably trying to add a fillet. You may also try trimming away the stem and lofting between the two halves. Use the tangent option on the edge of the trimmed surfaces and the stem will fair nicely.

    Your process is pretty much the same as I use, i.e. use the hull wizard to get in the ballpark then add detail features such as fillets, offsets, etc. in SolidWorks. Importing as 3dm will allow you to tweak the Rhino model and have those changes update in SolidWorks. Usually when doing that, your features will fail, but you'll just need to edit one or two to get it straightened out. It's not usually a big deal.

    I'll send you the model this p.m. CST.
     
Loading...
Forum posts represent the experience, opinion, and view of individual users. Boat Design Net does not necessarily endorse nor share the view of each individual post.
When making potentially dangerous or financial decisions, always employ and consult appropriate professionals. Your circumstances or experience may be different.