CAD Standard for 3D Data

MLombard
Retired

CAD standards have come a long way in the last 30 years or so. For 2D data, standards used to be mainly about layers and colors, and font size, and how to set up a drawing so it could be printed properly. The standards really demonstrated that even though you were now working on a computer to create nice drawings, you were still very much connected to the "old" manual drafting mindset. You were no longer worried about lead types, or ink, or pen nibs, but some of the details about construction geometry, line types and widths, and lettering were still there. The 2D CAD standards were to me the real proof that early 2D CAD was just a better pencil (or maybe more accurately a better eraser).

 

I still remember the laments of the old board drafters that all the personality and style would be lost with the new-fangled drawings. And they were right. But drawings weren't the end product, "the product" was, and personality and style - while a lot of fun, and very personally fulfilling - weren't necessarily helping you manufacture a great product. Not that electronic 2D drawings did much in that line either, aside from allowing you to make and correct mistakes faster.

 

So CAD evolves and now we still make 2D drawings, but we make them from 3D models. Making 2D views from 3D models makes the drawings more consistent (no manual projection mistakes) and much faster. Also more detailed, because the detail can be put into any view for free. CAD standards are still mostly about 2D. The 3D model is largely seen as a means to an end - in some cases its just throw-away data.

 

Model-based-definition (MBD) has been around for some time, but companies are paying more attention to it these days. We are still using 2D drawings, but in some cases, the 2D is just for visual identification and overall checks. More and more, things are going digital. You send 3D data to your machinist, maybe with a drawing that calls out only finishes and tolerances. You send 3D data to the molder, who again sends 3D data to be machined or EDMed, and again with a 2D drawing for overall weight, critical tolerances, and finishes.

 

If your operation looks like this, then your 3D data is more important than just something you make 2D views from. Your 3D data is probably revision managed just like your 2D data. And now, your 3D data needs standards just like your 2D data, but even moreso, because the way the data types are used has switched. 2D used to transmit part dimensions through someone who read the drawing and transferred the data to another machine or setup. Now those dimensions are automatically read in through the 3D data transfer.

 

So what kind of information should your 3D data standard control? In the days of history-based CAD, your 3D standard had to include best practice information, and in some cases had to go beyond just suggesting best practices, but had to directly specify techniques that users could and could not use. Standards and best practice are not the same thing. Standards must be followed. Best practices are usually set up as suggestions. However, standards can draw from best practice.

 

I've written 3D standards for history-based modeling, and I've got to say that they are very different from what I envision for a 3D standard for use with Synchronous Technology. The goal of the standard is to make your CAD data as re-usable as possible. You want to be able to use CAD data created with drawings in mind for other things like renderings, FEA, motion studies, assembly instructions, maintenance manuals, and any/every other place where your company uses graphical product representations.

 

If you are researching this topic, the one place I would start would be at http://www.resilientmodeling.com/01_SolidEdge_Home.html . I've mentioned this site before, and even Dan Staples gave it a thumbs up. The author of the site, and inventor of Resilient Modeling is Dick Gephard. His main aim is for companies to use this method as a CAD standard. It's worth your time to read through the entire Solid Edge portion of his site. Even if you don't use his complete idea verbatim, it still has great value for creating highly reusable CAD data.

 

The basic idea can be applied to any CAD system, but it has particular strengths when applied to Solid Edge in an Ordered/Synchronous hybrid work flow. The main body of the part is modeled in Synchronous, and the detail features are left in Ordered. Editing at the assembly level is done in Synchronous.

 

So what would I put into a 3D CAD Standard for a company using Synchronous?

  • Basic prismatic shape of part is always synchronous
  • interpolated (lofted) shapes must be ordered
  • use synchronous features when possible (patterns, holes, thin-wall, etc)
  • detail features should be ordered (fillets, chamfers, extruded text, etc)
  • use feature recognition tools on imported parts
  • avoid inter-part relations in assemblies, prefer synchronous edits between parts
  • geometry should be modeled at nominal sizes/positions unless you have a specific reason for modeling to MMC or some other condition.
  • versions of parts for downstream applications such as FEA or rendering should be handled in a separate FOP instance to avoid clashes with the instance used for the drawing

Of course file management is a separate issue that we can talk about later. The arguments around that subject haven't changed in recent decades, however. There are so many file management tools available for Solid Edge that it would be difficult to make an assumption about which one most people use.

 

I'm very interested in if anyone out there has written a 3D CAD standard for use with Synchronous, and whether you think it has succeeded or failed.

Comments
Esteemed Contributor

One thing that many folks might not think about is making similar parts oriented identically in relation to the coordinate systems.  This is critical if you routinely replace parts as having their orintation identical greatly improves the odds of having assembly relationships survive and accurately re-attach to the correct geometry.  Take a bolt for instance.  If the shaft followed the Z axis in one model, and it is replaced with another that has the shaft following the X axis, then you are relying greatly on the logic in Solid Edge to figure out how to flip it correctly and re-apply and relationships to similar faces.  The more complex your parts are, the more guessing Solid Edge has to do, and the chances it guesses wrong go up.  Having them oriented identically when modelled removes a lot of that guess work and improves your odds of a perfect replacement.

Retired

Yes, good one. Thanks!

Phenom

Along the same lines as Ken's comment- When making edits in a synchronous part, move a face wherever possible instead of consuming it in synchronous. Once the original face is gone, any assembly relationships based off of that face or its keypoints is broken. 

Phenom

(view in My Videos)
Great thread!

 

I have some questions. Would you eleborate on why you made each of the bullet points. Here are my thoughts

 

So what would I put into a 3D CAD Standard for a company using Synchronous?

  • Basic prismatic shape of part is always synchronous. I'm not working this whay, but I can see the advantages. Imported parts can be used, and more freedome to edit the profile.
  • interpolated (lofted) shapes must be ordered. Not sure about this, I don't do much lofting.
  • use synchronous features when possible (patterns, holes, thin-wall, etc). Not sure about this either, I'm using ordered.
  • detail features should be ordered (fillets, chamfers, extruded text, etc). Why is this one the opposit of the last one?
  • use feature recognition tools on imported parts. This is a procedure, not a standard.
  • avoid inter-part relations in assemblies, prefer synchronous edits between parts. WOW, I'm the compleat opposit.
  • geometry should be modeled at nominal sizes/positions unless you have a specific reason for modeling to MMC or some other condition. I compleatly agree
  • versions of parts for downstream applications such as FEA or rendering should be handled in a separate FOP instance to avoid clashes with the instance used for the drawing. What is an FOP?

Of course file management is a separate issue that we can talk about later. The arguments around that subject haven't changed in recent decades, however. There are so many file management tools available for Solid Edge that it would be difficult to make an assumption about which one most people use.

 

Question: Besides the revision manager, how can I move a group of linked files while maintaining all the links?

 

I could be an ecception to the rule as I have to coustom size each produced product. The details don't change, jsut the overall size. I have to be able to resize about 10 sheet metal tanks a day.

Phenom
  • use synchronous features when possible (patterns, holes, thin-wall, etc). Not sure about this either, I'm using ordered.
  • detail features should be ordered (fillets, chamfers, extruded text, etc). Why is this one the opposit of the last one?

It is not, and the reasoning becomes clear if you have ever had to do synchronous edits on a part with a large amount of fillets/chamfers. Because features like fillets/chamfers/extruded text consume the original faces they are placed on, it becomes exceedingly difficult simply to get back to the original design to make an edit. By constructing the majority of a model in synchronous, and applying these other features at the end in ordered mode, you are using the best of both worlds. You still have the ability to quickly and easily make complex edits to the shape in synchronous, while retaining the ability to roll back your chamfers or reapply them in ordered, with neither affecting the other. This also follows the doctrine of 'Resilient Modeling', which is supposed to help you build models that react well to edits. There are many youtube videos and other articles on this subject. Here are a few:

 

http://www.design-engineering.com/cad-cam/using-synchronous-and-ordered-modeling-in-solid-edge-86414

http://ontheedge.dezignstuff.com/chew-on-this-resilient-modeling/1536

http://community.plm.automation.siemens.com/t5/Solid-Edge-Blog/SEU14-video-Introduction-to-Hybrid-Mo...

 

 

 

  • use feature recognition tools on imported parts. This is a procedure, not a standard.

Ketchup, Catsup

 

  • versions of parts for downstream applications such as FEA or rendering should be handled in a separate FOP instance to avoid clashes with the instance used for the drawing. What is an FOP?

Family Of Parts is a collection of parts of similar size/features, with family members driven by a variable table.

Esteemed Contributor

And instead of using FOP (Family of Parts) if you only need one other instance of a part that is "de-featured" or has additional features, just use Insert Part Copy.  Result is two files instead of three...

Phenom

Starting with the first line item "Basic prismatic shape of part is always synchronous"

I have encountered problems with that because is impossible to create 2 way and 3 way corners sheet metal part in sync alone when there is no references geometry. Sync needs to temporarily allow overlapping flanges to get designs started.

 

That alone has prevented me from using Sync.

Retired

Yeah, sheet metal has some special circumstances. Every release, new situations are handled.

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