Using Prochine and Solidworks together.

Hello:

I really enjoy all of the information dispensed here. Been looking for a couple of weeks, and it was time to sign up and join in.

I am working on designing a 21 foot jet boat. I am using New Wave Systems Pro Chine for the hull and have a design that I think is fairly close. (It is fun to print out the flat patterns on the inkjet, tape it all together, and show it to friends and co-workers for a critique.)

My plan has been to get a hull shape I am happy with, generate an IGES file, and use Solidworks to generate the rest. I am somewhat proficient on both programs, but have little experience with surfaces in Solidworks.

Any advice for someone just getting started? So far I have:

Generated a developable shape on Pro Chine.

Saved an IGES file for each surface.

Imported the surfaces into Solidworks.

A specific question I have is what to do with the surfaces in Solidworks. I am used to working with solids and so the first thing I did was try to generate a solid out of the surfaces using the thicken command. The bottom surface worked fine but the side gave an error. The message only said “unable to thicken surface”. So, should I be trying to turn the surfaces into solids? If so, any ideas on the best way to get Solidworks to cooperate?

Andy Hanna

 

the idea for thicken the surface is just to have a solid that can have a volume that you know, but:

1) You must find why the surface won't work, because is the right thing to do, that way you know what the software is capable to do and what not or why.

2) I don't use solid for my hull surfaces, all my information in weights go to my spreadsheet, so they really don't do much, I don't trim the surface in any way, I don't trust trimmings in any software,( for surfaces). so I try to keep my surface the most intact that I can.

3) I use Prosurf too, so I create the hull there and finish it in rhino and then goes to Solidworks as an iges, so from rhino I get all the cut outs in the hull, bulwarks and deckhouse, but again I try to do the least trimming.

And thinking about that surface that didn't thicken may be related to the way the surface is defined, is a surface with tons of control "points or vertexes", that may cause that when you thicken the surfaces the vertexes try to overlap so the thicken option gets wacky and fail.

let us know how it goes, and if you were able to find the answer to that

 

Andy-

I use Proline Basic to design both round bilge and curved hulls and export IGES surfaces for further work in Cadkey 21 (Acis solids and surfaces). I don't know if these comments apply to Solidworks, but here are some issues and workarounds I've used when trying convert surfaces to thickened solids:

If your lower chine edge or fairbody edge curves to meet the stem edge tangentially, the surface may develop anomalies right near the intersection. When you try to thicken the surface or create an offset surface in your solid modeler, it tries to create points for the offset surface directed along the surface normal - the cross product at the UV curve intersections - and can't accurately determine this if your chine curve blends into the stem curve. try creating a sharper corner here in Nautilus and trimming it to final profile after you've generated the thickened surface.

Also, examine your surfaces in Nautilus and test for Gaussian curvature using a high density color patch, looking paricularly at the corners. Be sure your surface is really close to developable. If you have spot of great color gradation at one of your panel corners (local compound curvature), it can cause all sorts of grief if you try to create a thickened surface solid due to self-intersections. ProChine should have options to force a patch to be developable or you can manipulate control points until you get a developable surface.

Sometimes I can't create a thickened surface in Cadkey, but can create an offset surface, then add ruled surface around the perimeter and then convert that to a solid. If it becomes to big of a pain, I just stick with surfaces and offset surfaces and don't expect perfection. Good luck.

Chris Krumm

 

Try useing the knit surface command in SolidWorks before you thicken. This usually works if the surface(s) is clean.

 

So here is what I have found out so far.

When I was working with the ruling lines I had left the bottom of the boat as a Vee. I had intended to add a "ski" for the jet unit after all the shaping was done. I had used a hard knuckle point on the curve where the boat transitioned from the almost straight aft section to the forward section. When you convert the ruling lines to surfaces the knuckle is not transfered to the surface. When I added the ski it produced an odd little wrap in the surface just forward of where the knuckle used to be.



This is the overall view of the boat. (I hope)



And here is the wrap.

Once I fixed the wrap, by putting a knuckle in the surface, I retried the Solidworks thickening command. Still didn't have much luck but now it was the bottom skin. I looked it over and I think it looked ok. There were a couple of spots that weren't perfect but not bad.

Played around with it a little and it turns out it made a difference which hand of the boat I was working on. Some skins would work on the left side and some would work on the right. So some trial and error and judicous use of mirroring allowed me to produce a complete solid.

Thanks for all of the help. With the surface to solid transition.

So I guess I am less confident about slicing things up in Solidworks to produce my frames, front deck, and gunnels. Would I end up with more accurate results taking the cuts in ProChine?

CGN: It sounds like you do a lot of suffling between programs. What does Rhino do that Solidworks is lacking and when do you slice up your skins to produce the interior structure?

Chris: I think the problem was similar to your prediction.

I looked at the Gaussian curvature in ProChine and it looked OK, maybe I need to zoom in and get a little more picky. I will go back over everything closely. Do you use Cadkey to generate your interior structure or do you use proline basic?

Doug: I did investigate the knit command, but it is used to join two surfaces. I was afriaid to use this because I didn't want to change the shapes of the surfaces. And from reading about the command in the help section I did not think it would help. Am I wrong?

Thanks again everyone.

Andy Hanna

 

Hi, glad to hear that you are into that, and finding some details to improve your models, I won't model a boat surface with so many vertexes I will use k-patch to check my curvature and if I have to pay the price a little bit of curvature in my plate just to avoid that many vertexes, but that is another topic, what I been doing to get in solidworks the frames is the next process:

From the beginning:

1-Create the hull surface in prosurf
2-Export to rhino and finish my model decks, deckhouse, transom etc..
3-Export to solidworks as an IGES and create an assembly file with the hull surfaces
4-Create reference planes where my frames are going to be located

here I will go to specific what I do to create the bottom frame made of 4"X4"X3/8" angle just to name a profile size.


This is from tech tips for solidworks, you may now this one by now

1-go Insert -> Component -> New sequence is a convenience feature to save the user several steps. The most general, un-constrained method to add a new part 'in context' is as follows:
1) Use the New icon to create a new, empty Part.
2) Save the new part with some appropriate file name
3) Add the part to the assembly. You could do this via the menus, (Insert - Component - From File), or you click on the top-level icon in the empty part's Feature Manager, and drag it into the assembly.
4) Create whatever Mate relationships are desired, using either the origin or any of the starting planes of the empty part.
5) Right-mouse click on the node in the Assembly's feature manager that represents the empty part. Choose the function Edit Part.
6) Pick a plane or face and open a sketch to serve as the base-feature of the new component.
Now go to town, sketching and building features just as you would have before.

You have just duplicated the functionality of the Insert....New function, with the important difference that you have not yet created any "In-Place" mates and have instead located the new part using one or more mates of your own choosing.

2- ok you choose the first "frame" which is your first plane and you inserted the "part" name it "Fr-1" and insert an sketch.

3- here is the trick, use Tools- sketch Tools- "intersect curve", and then you have the frame moulded line, finish your sketch.

4- create a plane "normal to curve" in any side of the curve.

5- now on this plane I sketch the angle and the use the sweep command, check
"no merge"

6- there is the bottom frame at Fr-1

I don't cut sections on the boat, I use intersection curve if is a full bulkhead for example I do step 1 and 2 and instead of only intersect the bottom I intersect bottom, side and deck.

I don't thick my surfaces and I don't trim surfaces or I tray to avoid it, you can roll or develop a surface with all the trims marks on it and once you have it flat just trim in 2d and leave the boundary to be cut.

why prosurf-rhino-solidworks?

Prosurf you know why, Rhino is not better than solidworks, and solidworks in no better than rhino the two of them are good on their area I like to have rhino besides to be easier to work surfaces than prosurf and solidworks, I can expand my plates here with Expander, double curvature or developable surface is not that prosurf can do that, is just that I can work my surfaces, intersections and renders in rhino way better.

so surfaces in rhino structure in solidworks.

no slices, no cut of the hull, just the full surface

I hope this can help, please if you have more questions i'll be glad to help.

 

Andy -

I have used ProBasic with Cadkey to design several hulls, the largest being a 24'-8" round-bilge trimaran that I have female moulds for Vaka and Amas prepared for. All interior structure has been done in Cadkey as surfaces and solids. I ported in 1/2 hull surface and faired profile curvesfor stem, cabin and decktop, and transom from ProBasic. I thickened the hull surface into a solid based , trimmed to centerline, and mirrored. Final deck surfaces and solids were lofted thru 3 -point arcs from sheer-centerline-sheer.

I typically model my hull surfaces in ProBasic projected to the centerline at the bow with an obvious acute angle where fairbody meets stem, then trim surfaces back to a final stem profile curve with a radius blending radius fairbody-to-keel in Cadkey prior to thickening the surface(s). This gets rid of the little "warps" prior to creating a solid, and also gives me a stem that transitions from very thin at the waterline to bluff at the stemhead.

My ProBasic surfaces run wild at the transom and then trim and generate transom surfaces or solids in Cadkey. Again, I like to use ProBasic to give me fair curves to use as trimming guides in Cadkey. My version of ProBasic only exports curves as DXF polylines, so I use tools in Cadkey to map 2D spline curves over them.

Have had no problems with accuracy of section cuts through the Cadkey solids and surfaces on any plane. ProBasic/ProCHines seems like a confusing place to work out and store all that information, especially for a larger boat. My biggest problem is trying to model beveled, twisting solids for stringers, gunwales, etc. in Cadkey. Here's where I quickly start thinking "this is fun, but let's just skip it and build the damn boat." Suppose getting that all sorted out on the computer would be advantageous if you're trying to do a bunch of CNC notching into panels for framing members.

I have built 2 hard chine sea kayaks ( 1 ea. 4 panel and 1 ea. 8 panel hull) and one round bilge version of the 8 panel hull using ProBasic and Cadkey. I relied on ProBasic for all the flat plate developments and most of the bulkhead plots 'cuz I didn't feel it was worth much time working detail out in Cadkey. The ProBasic plate developments and bulkhead patterns (with skin thickness deductions) were dead nuts on for these projects.

Sorry for the long post. Good luck on your project, and I'd welcome any opinions on Solidworks - several friends are extolling it's virtues.

 

Hi Kris now i have a question for you, how do work with cadkey?, is stable?, it's memory hog?, i ask you becouse use solidworks at work, and i'm looking for a system for me i like solidworks or Pro E but cadkey seems to me like a very complete package becouse you can get 2d drafting, parametrics and surfaces for a good price specially now that was bought by this new company, i will like to hear your opinion.

and about solidworks, i can tell you that really works good and i mean stable, lean and clean interface if you were user of autocad, solidworks feels like it very robust.

Thanks

 

CGN

Started using Cadkey years ago as a version because it was an inexpensive , easy to learn, fully 3d capable wire-frame CAD program with a good surfacing plug-in (the old FastSurf program). Annual upgrade contracts were relatively inexpensive, though I feel they were often late and promises were made in advance that were'nt kept regarding features and "bug-freeness." They were on to the next version, with more bells and whistles, before fixing some basic glitches were forgotten or were advertised as a new "feature" for the newest version. Nothing really onerous here - lots of software companies seem to operate this way.

Parametric add-on was never purchased so can't comment on its capabilities, other than to guess my interest in it would be limited to wanting it sort of optional; i.e, to be able to modify a surface by revising the parent curves, with the option of not having to always build models parametrically. I'd welcome more info on how rigidly it is enforced with ProE or Solidworks.

The latest version of Cadkey, 21 and 21.5 has assemblies, and it was long overdue. Version 19 was stable, but having to keep all the geometry in 1 file made for some serious memory issues. Layout mode, analogous to Acad's Layouts or old Paperspace, worked pretty well. I had some misgivings about it's ability to cut sections and to render 3d wireframe hidden line views - very slow and prone to representing spline edge curves that looped around the page, and required manual clean-up. Quite often I end up creating non-associative sections for very complex part assemblies, either by cutting the section and saving the view to a level for clean-up; or by copying the geometry, trimming to section planes, and creating ortho views of that copied geometry. Of course, associativity is blown. 21.5 has exploded view capabilities. Includes a nice package of fasteners, structural sections, etc., available as 2d or solids.

Dimensioning and annotation capabilities are complete, though not to the level of AutoCad. Can't dimension isometric views in Layout mode - an oft requested feature in their user forum. Wish you could customize the program with VB and Active X type controls, but the macro programming is easy to learn.

ACIS solid modeling and surface generation in 21.5 are is complete, making it a good value. Imports IGES and SAT files with minimal fuss and does pretty well with DXF. From what I can see on the change to KeyCreator, you're going to basically be working with Cadkey 21.5 for the near future, and they're going to push the integration with the 2d and 3d NC plug-ins Cadkey started to work on in the last couple of years. It's biggest plus was/is still ease of use. A lot of [former] coworkers in the exhibit design industry extoll Solidworks or ACAD Mechanical desktop, but for the price and ease of use, people learned to model and create shop drawings proficiently with a short learning curve and at a much lower software price point. All that said, I'm not married to it...

Chris Krumm

 

Thanks Chris, it really helps me your comments about Cadkey, now about solidworks, solidworks itself is "good" with surfaces but seems that free surfacing is coming form plug-ins for this task, there is surfaceworks, which is an extension from multisurf really well known hull design software, they are parametric since the beginning but I remember was tricky to work with, so I never really started with it, and there is a new free surface software a plug in for solidworks for surfacing too, like you see I'm not really into surfaces for solidworks and the reason why I haven't been so interested in learn to use surfaces in solidworks is because is very well integrated wit rhino, from solidworks you can open native rhino files, and update surfaces which is good enough for me now.

 

CGN and Chris:

Been negligent getting back to you guys. Been so busy, I haven't had a chance to try any of your suggestions.

In re-reading the thread I noticed I neglected to mention that I intend to CNC cut all of the pieces. And that if things go well, I may try to offer a kit for sale. That is why I am being so picky about getting all of the geometry correct in the computer.

I have decided that I need to redo all of the lines on the boat. In laying it out at first I used knuckle points in the transition from the straight aft to the curved forward. This caused a lot of trouble and needs to be changed to a full curve.

I will try to get some time in this weekend on the project, but with the boat show in town and a friend moving, I think it is wishful thinking.

Thanks again,

Andy Hanna

 

Andy -

After looking a litle more at your attched JPG files, I have a couple questions:
I use ProBasic, so I can do both round bilge and hard chine hulls, but I thought I rmember ProChiines being a subset of ProSurf/ProBasic. With that said, It looks like you are designing a fairly straightforward 2-panel hull, without any weird steps or strakes.

From your JPGs, it looks like a lot of control points defining fairly simple chine curves, and from the detail shot, it looks like the upper surface control points don't align with the lower surface (I'm assuming all the sqauer points are your editable control points. Are the two surfaces bonded along the chine, and how were they orginally created? MAybe I'm missing something in your design or how ProChines works compared to ProBasic, but just my thoughts.

The chined hulls I've drawn - some with spray strakes, but none with transverse steps - have used maybe 10 columns max, and chine curves have always been bonded. Have had little trouble creating clean thickened-surface ACIS solids from them.

Chris Krumm