Ship/Yacht Design with Inventor

[jdchakes]

Hi

The Company I am at uses Inventor for ship design. All kinds and sizes of boats.

Im just wondering about other peoples experience using the software for this purpose?

Am looking to start a discussion based around Inventor and ship/yacht design.

The rough outline of our current approach to a design is to import our hull surfaces into a part file, this becomes a multi-body part file with the base structure, BHDs, Girders, stiffeners. (this part file can get very large so create serpeate files for seperate ship modules: forebody, skeg, wheelhouse etc.)

Then derive parts using 'make components' to create a final structural assembly.

We then detail these individual components within the assembly and ad the simple structure such as brackets to this assembly.

Then have other assemblies with machinary, deck gear, fitout etc.

The main problem I have with this approach is getting out the final cutparts, long tedious manual task of exporting shapes to autocad, i'm sure there would be a more efficient way to create and name cutparts using iLogic?

Another task I am looking at doing is using iLogic/VBA is to colour the assembly based on plate thickness?

Any and all feedback would be greatly appreciated.

Cheers

[tmoney2007]

If some of the parts are sheetmetal, you can definitely automate exporting the flat patterns for these parts. I think there might even be something in the autodesk store for it. My company primarily fabricates sheetmetal parts so we've automated this pretty extensively because our volume is huge.

For other parts, if you use an inventor DWG as your drawing format, they can be opened in AutoCAD, or you can set inventor to save a DWFx (I think) and the shop personell can open those in Design Review.

As far as automating the creation of flat drawings from your parametric parts, I'm always leary of taking the human element out of dimensioning, but a script could probably be written that would create an IDW or DWG for each part and subassembly and place the base views. The usefulness of this will depend on how consistently the parts are created. If the users always create their parts oriented a certain way within the coordinate system of the part file, it will be much easier to get something useful out of this automation, otherwise you'll tend to get a drawing file with a view that usually gets deleted.

[jdchakes]

So the way to somewhat automate cutparts using the top down modelling approach may be.

1. Create large multi-body part as usual
2. 'Make Components' to create individual parts
3. iLogic code to identify plate thickness of part, and convert into sheet metal part
4. then use iLogic to automate naming of the cutparts
5. iLogic to take all same thickness parts and dump their shapes onto the same dwg/idw and place a label on each part

Im not so concerned about dimensioning and laying out drawings, this can be done manually.

Im looking to automate, to remove human error in duplicating part names, missing out parts, applying wrong thickness etc.

I see you can get/set sheet metal sytle and get its length, width area etc. My main problem is getting the thickness of the solid body in my original part, i cant find any parameters in the ilogic wizard to use (see the attached image). I can see the derived part and which solid body of the part is being used, but not any paramenters (e.g. thickness) used to create that solid body?

Any help would be greatly appreciated.

Thanks

[rjay75]

Are they all different thicknesses? Are there any other properties on the parts such as a specific material style, part number, stock number that you can get the material and possibly know a thickness for?

If there are nothing on the parts to determine this another option would be to programmatically cycle through all the planar surfaces and see which two are the largest and closest or equal in size (countersinks and counter bores may make the two sides not be equal in area). Then get the distance between the two if they are parallel to each other. The distance should be a usable thickness.

I actually use the sheet metal environment for any part that I need to get flat pattern shapes from regardless of the material it is specifically for the purpose of get the flat pattern and being able to mass export flats later. Also if the part is going to stay flat or be bent with a uniform thickness the sheet metal tools help a lot to do that than conventional modeling.

[tmoney2007]

It might just be our setup, but I think that sheetmetal parts require a system parameter called "thickness" to be set up. You can use that to drive the appearance via iLogic.

[rjay75]

When a part is converted to a SheetMetal part the Thickness parameter will automatically be created. However if the value of the Thickness parameter doesn't match the uniform thickness of the part then none of the sheet metal commands will operate correctly. And creating a flat pattern will not operate at all.

So even though Inventor will create the required parameters for the sheetmetal environment the Thickness parameter has to be set to the actual thickness of the part.

[Pontooon]

Check out widom tech woodworking for inventot

[jdchakes]

Ok so sounds like the best method is once the solid bodies have been made into individual components, convert each one to a sheet metal part. then in the main assembly, write an iLogic code that will go through and colour all the parts based on the sheet metal thickness parameter.

[theo.bot]

Hi,

We talk with our customers about digital shipbuilding. We use autodesk products and specialized shipbuiling software based on autodesk for ship building. We position autodesk inventor for equipment design. We use ssi shipconstructor and autocad for the structure design and piping.

Check the site of ssi for more information: http://www.ssi-corporate.com

If you're located in the netherlands you can contact us directly: www.cadmatch.nl

But, off course you can use inventor for the design. But in many cases you have to find workflows and workaround for specific needs.

Kind regards

Theo