How to send out un-editable assemblies to customers? 2

[BrianE22]

I'd like to make available our product as an assembly to users but I don't want them to be able to edit or take apart the assembly. This is for them to put our assembly into their Solidworks files. What is the best way to do this?

 

[MikeHalloran]

I used to work on Diesel generators, and got fairly detailed files from the engine manufacturer.
The interior of the engine was greatly simplified; e.g. the camshaft and crankshaft were represented as straight cylinders, with correctly detailed flanges at the exposed ends.

The models were supplied in some 'neutral' format that I don't recall, that could be imported to SW, and were detailed (on the exterior) right down to the split lockwashers.

... which were a huge problem, because the angled split surfaces came into SW as some sort of Mobius Strip like entity that caused SW to choke, so you had to replace each and every one of the damn things with a better model before SW could use the assembly.

I suggest you do something similar, e.g. supply a 'dumb solid' model of all the exterior interfaces, omitting the interior intellectual property or greatly simplifying it. ... and supply a simplified model of any lockwashers as well.




Mike Halloran
Pembroke Pines, FL, USA

 

[JMirisola]

Take a look at 'Defeature' located under the tools tab. Check out this blog post that describes how to use it:

http://blog.capinc.com/2012/04/how-to-simplify-assembly-geometry/

Jeff Mirisola, CSWE
My Blog

 

[CorBlimeyLimey]

Use the Save as function to save the assy as a part and use the Exterior faces or Exterior components option.

http://help.solidworks.com/2014/english/solidworks/sldworks/c_multibody_parts_vs_assemblies.htm

 

[Jboggs]

I thought that was what E-drawings was for. You can open files, but not edit them. And its free.

 

[GRF]

I have had good luck using the following process.
1. Export assembly as a .stp file into a new directory.
2. Open the .stp assembly.
3. Save the assembly and files in Solidworks format
4. Select one of the files and edit it in the assembly.
5. joint all other parts in the assembly to that one part.
6. Save the part
7. open the part and fill all the empty areas so your customer cannot figure out what is on the inside.
8. Save the new file.
9. Export to .stp again (need to do this so if you send the file out as a Solidworks file they cannot delete your
10. Open the file and save as a part file.
11. Either send out as a part file or convert it to another solid type.

This can be a relatively long process but it does ensure that people only can do a form fit with your model. Everything is one solid part and since you filled the inside they have no idea what the inside is.

 

[ctopher]

I do the same as what CBL and Jboggs suggested.

Chris, CSWA
SolidWorks '15
ctophers home
SolidWorks Legion

 

[BrianE22]

Thanks for the ideas everyone. I'm going to have my CAD guy try each of them. I don't think E-drawing would work unless Solidworks can import that format so the end user can move around and rotate the product in their Solidworks files.

My current customer was o.k. with a .STL formatted solid so I'm o.k. for now.

 

[Jboggs]

BrianE22 - Edrawings is a Solidworks product, made specifically for the purpose you asked about. It allows your customers or others to view SW files (3D or 2D) with free downloadable software but will not allow them to edit the files. Check with your SW reseller or their website. So of course SW can import Edrawings files.

 

[CorBlimeyLimey]

JBoggs,
I think the point BrianE@@ is trying to make is that an eDrawing file cannot be inserted into other SolidWOrks files (part or assembly). ... to check for fit/clearances/etc, or simply to complete the final assembly.

 

[Jboggs]

CorBlimeyLimey, I stand corrected! I learned something here today. I saved a SW assembly as a E-drawings file. Could not open that file in SW! Opened it in E-drawings. Could not save it as a SW file or anything SW can open. That is weird and makes no sense to me.

 

[TheTick]

I now all too many CAD designers who regularly produce unetitable work. Maybe one of them can help?

 

[CorBlimeyLimey]

JBoggs,
The eDrawing program is just a viewer for SW files. It allows customers or other departments to view, measure, red-line, etc, SW files without needing SW installed.
It can also save as STL.

 

[MikeHalloran]

eDrawings allow viewing, but not comparison/ fit checks/ insertion/ union/ intersection/ difference checking.



Mike Halloran
Pembroke Pines, FL, USA

 

[DiegoLGraves]

TheTick - too funny!
I do what CBL suggested, saving the assembly as a part with just exterior faces. If the weight is important to the user I may also adjust that before sending it out.

Diego