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Merge, Inheritence, Copy Geometry and Publish Geometry


Merge, Inheritence, Copy Geometry and Publish Geometry

I am always confused that what is difference between Merge, Inheritence, Copy Geometry and Publish Geometry features. It seems the function of all three are same. When we should use which feature? Thanks!
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Publish Geometry is a way to bundle together geometry in one part for easy reference by another part. It is used for Copy Geometry features, to re-use geometry in another part as reference. By using Published Geometry, you make it simple and fast for others to select the correct items when using Copy Geometry. Otherwise, there is the possibility that different people could grab different (incorrect) reference geometry. Copy Geometry allows you to grab features and refrences from one part to use in another part. It is indispensible in Top-Down design, where you want separate parts to share common references. In my case, I can use Copy Geometry to grab the internal surfaces of a cast part and incorporate them into a separate part that represents the 'core'. Once the surfaces of the inside are in my new part, I can close them and 'Solidify' to make a representation of the 'core'. Merge/Inheritance is the way you incorporate one complete solid part into another solid part. Merge inserts a monolithic solid feature representing one part in another part -- no changes allowed in the new part. Inheritance does almost the same thing, except the solid feature is not monolithic, you have access to the individual features and therefore you can alter the Inheritance feature in your new part. We use Merge/Inheritance to handle cast and machined parts. Part 'A' is modeled as a casting. Part 'B' is created to represent the "as machined" version of the casting. Inside Part 'B' insert a Merge from Part 'A'. Once done, we can now make cuts to represent the machining operations. If we then change the casting (Part 'A') those changes ripple into the machined casting (Part 'B'). Merge also allows you to make a mirrored copy of a solid part. This came in handy once when we had a design with a left-half and a right-half. We modeled the left-half then used the Merge (with mirror) to make the opposite. Merge will also allow you to make Cut Outs. We have used this functionality to make assembly nests or other such fixtures. Simply make a block of material in Part 'B', then Merge/Cut out Part 'A'. Inheritance is relatively new. I haven't used it. But it seems ideal for cases where you want to to model a part that is a lot like a previous part, but you want to make subtle changes in dimension. I can imagine this would be the case if you were making a new pistol and wanted hand grips almost like another model. You could inherit the grips, and then alter dimensions to make the new grips fit a wider hand (for example). I'm sure PTC can offer other, better examples.

Thanks John for such a detailed explanation. Can u plz give example where we can use Publish geometry.

Great post John, I hope I don't mess this up and confuse the issue. I think I'm correct in saying that you don't directly use Publish. What you do with publish is set up what you want to use, both for other users and yourself. Then when you want to use that particular configuration you can copy geom --> use published geometry

Published Geometry finds its greatest application in Top Down Design (you'll have to contact your PTC training guru to help you with this very complex concept). I will try to give you a flavor here. Suppose you have an assembly concept that will involve the interaction of 5 separate parts. Traditionally you would have to complete the design of each of these parts and them assemble them together. Also, in the traditional assembly scheme, the parts will reference surfaces of the other parts, creating multiple parent/child relationships. This won't become a problem until you have to change some of the parts. Then it is very likely that the assembly regeneration fails because the necessary reference feature(s) is no longer available (perhaps draft was applied, or a cut was made that eliminated the surface). The solution is to create a 'Skeleton' part. This part only contains datum planes, or axes, or other reference surfaces. Its purpose is to provide a scaffolding onto which you assemble your sub-parts; you can also define a 3D boundary using surfaces to act as a "space claim". (Then, by agreement, parts must remain entirely inside the boundary to be sure no interferences arise.) Since the sub-parts only reference the skeleton, you avoid the parent/child relationships between sub-parts. You can also assemble the sub-parts to the skeleton before any solid geometry is made (if you take care to define the datum interfaces beforehand). Then as you design your sub-parts, they are already in the assembly, properly located, and you can see how everything is fitting together. You can define common datum features in your skeleton and then share these to all the sub-parts using Copy Geom. Here is where Publish Geom really comes in handy. Inside the Skeleton, collect all the references to be shared into a Published Geom feature. Then when in the sub-part, Copy Geom and select the Published Geom feature. If you have multiple designers working in parallel, it is much simpler for them to grab one Pub Geom than try and pick all the correct individual geometry themselves. You really need to consult your local PTC rep and take the Advanced Assembly course to completely grasp this great design style. I simply cannot do it justice here. Good luck.

quick question John, you say you can copy geometry to make a core. My copy geometry button is blacked out. Do you make a quilt first or just select surfaces? Anything I try doesn't allow me to copy geometry. I want to make a seperate solid of the core area just like you said but I can't save just the core area. Any help would be great. Thanks Daryl

Another question John, your skeleton file is it the top level of an assembly, or is it a .prt file that is the first file in an assembly. Thank you Ian

If Copy Geometry is greyed out you probably don't have the Advanced Assembly Extension or it could be that the license file you have doesn't have the option. Skeleton part files are placed at the top of the assembly. The file is not created using the the new file dialog, it's created in assembly mode. When you have an assembly file active use the Create (Create a component in assembly mode) icon or Insert>Component>Create, Skeleton Model should be one of the types listed.

Just a thought. If you're using copy geometry without any published geometry, make sure you've unchecked the "published geometry only" icon. (Cube with three arrows coming out of it.) When I first started using there features, I always forgot to do this.

Is the skeleton part file only able to be created if you have the Advanced Assembly Extension?

Yes, I believe you need the Avanced Assembly Extension.

Yes, you need Advanced Assembly for full Skeleton Part functionality, namely having the system recognize the Skeleton part as such. However, this technique existed before it was integrated in this manner, and you can still do it "the old way" by building a regular part using Planes, Axes, etc. and assembling it as your first part. Trouble is, you won't be able to easily exclude it from things like a BOM or include "real" mass-bearing features and filter them out in the way you can if you have AAX.

Hi, this may seem like a trivial question, but how do I know if the published geometry needs updating? There aren't any prompts or symbols that tell me if the geometry has changed.

This instance arises when a colleage may be working on a component that I am using as my copied geometry references from on a different part.



You need to have the source part (with the public) in session and then regen the target (with the copy). This assumes it's an external copy geom, if it's a standard you'd need the parent assembly in session too.

Doug Schaefer | Experienced Mechanical Design Engineer