Converting Parts in Assembly to 1 Part

[PhillDavis]

I have a part that is constructed of several castings and extrusions that are welded together. I drew it as each individual component in an assembly, but I would like to turn all of the individual parts into a single part file. I can convert the assembly into an IGES file, then bring the IGES back into Pro E as a single part. But when I do this, I lose all of my planes and axis definitions. I can redefine them, but it would be much easier to just do the conversion within Pro E. Is there any way to do this?

[DavidButz]

Phill, The quick answer is yes. You can pick one of the parts and merge all the rest of them into it, or use a blank part and merge all of the parts into it. Use Edit/Component Operations/Merge. On the other hand, I am a little curious about why you are doing this in the manner you describe. Maybe you are using a creative and appropriate way of creating your part, but it strikes me as a little unusual; there could be other methods of modeling that would serve you better, but it's hard to know without more detail. David

[GrahameWard]

Component Operations>Merge is getting a little old hat these days. I used to use it a lot but would recommend Copy Geometry these days. If you don't have Copy Geom available you can use Copy and Paste across the assembly to copy solid surfaces from one part into another. If you need to copy lots of datum planes though you could be making lots of features. Also with this method you will need to go back to the parts to modify them.

[PhillDavis]

I am reverse engineering an aluminum motorcycle frame. It is constructed of 14 major parts, 6 extrusions and 8 castings. When doing the drawings, the extrusions are fairly straightforward and easy. But where I am having problems is when I draw the castings. They have different wall thicknesses, ribs, chamfers, rounds, etc. The problem is not with drawing the first piece of the frame, it is when I draw all of the succeeding parts. When I go to shell, chamfer, or round, I get into a lot of problems because the action I am trying to perform doesn't stop on just the piece I am currently constructing. For instance, a shell operation tries to shell the entire model up to that point, even though the previously constructed parts don't need it. Now I know that someone really proficient with such tasks could probably do it within a single part file. But for me, it just seemed easier to construct the model exactly as the original was constructed; one piece at a time. By starting as an assembly, then constructing each individual part within the assembly, it allowed me to more easily control the process and final shape of the individual parts. But now I am looking to bring the drawing back into a bigger assembly. Now I can bring the entire assembly into another drawing, but I am having problems with that as well. Whenever I insert an external assembly into another assembly, it works just as is should, until the next time I open the file. If I restart Pro E and try to reopen the parent assembly file, Pro E can't find any of the inserted assemblies, I have to go manually locate them one at a time. I don't understand why this is happening, because I can insert an individual part from an assembly, and it works every time the file is opened. But if I insert the entire assembly, contained in exactly the same folder, it can't find that.

[ReinhardN]

Hello Phil, you should dig in the help files for search_path. ProE looks for components in follwing order: - memory - working folder - search paths By the config option search_path you tell ProE where to look. HTH Reinhard

[ArisTroulis]

If I understand well from what you are saying, you have design intent problems. I think you have started to design an assembly by creating the first part and afterwards you continued designing part after part with reference to each other without considering any design intent methods. You cannot design parts in assembly by referencing from one to the other backwards and forwards!!! You get all sort of problems like circular reference errors etc. The best way is to assemble empty parts with the fist three datums and the coordinate system into the assembly and design the geometry of each part seperately. Afterwards you can put the apropiate values always referencing the first three datum planes with the assembly datums or to each other. In case that you need to fit components into each other "ie gears into a casing you import the casing geometry into the gear part as your first feature and use reference from the casing geometry". Always remember that if you use reference that they will change the other part that uses them will change also.

[DELETEME]

"Phill Davis" wrote:

I am reverse engineering an aluminum motorcycle frame. It is constructed of 14 major parts, 6 extrusions and 8 castings. When doing the drawings, the extrusions are fairly straightforward and easy. But where I am having problems is when I draw the castings. They have different wall thicknesses, ribs, chamfers, rounds, etc. The problem is not with drawing the first piece of the frame, it is when I draw all of the succeeding parts. When I go to shell, chamfer, or round, I get into a lot of problems because the action I am trying to perform doesn't stop on just the piece I am currently constructing. For instance, a shell operation tries to shell the entire model up to that point, even though the previously constructed parts don't need it. Now I know that someone really proficient with such tasks could probably do it within a single part file. But for me, it just seemed easier to construct the model exactly as the original was constructed; one piece at a time. By starting as an assembly, then constructing each individual part within the assembly, it allowed me to more easily control the process and final shape of the individual parts. But now I am looking to bring the drawing back into a bigger assembly. Now I can bring the entire assembly into another drawing, but I am having problems with that as well. Whenever I insert an external assembly into another assembly, it works just as is should, until the next time I open the file. If I restart Pro E and try to reopen the parent assembly file, Pro E can't find any of the inserted assemblies, I have to go manually locate them one at a time. I don't understand why this is happening, because I can insert an individual part from an assembly, and it works every time the file is opened. But if I insert the entire assembly, contained in exactly the same folder, it can't find that.

[HatimAbdul]

Phill: Back to your original question, I find the most effective way to achieve merging is by shrinkwrapping. From the assembly, #File, #Save a Copy. Choose "Shrinkwrap" from the "Type" list and enter a name. Then you'll get a dialog box to ask you about what type of expoting you want. In your case, you want "Merge as Solid" and specify a quality level (the higher, the slower). That will produce a Pro/E part combining your assembly components. Be aware that, because it's an external model, it's not associative to the assembly. So you'd have to re-export when assembly changes.

[PhillDavis]

"Phill Davis" wrote:

I am reverse engineering an aluminum motorcycle frame. It is constructed of 14 major parts, 6 extrusions and 8 castings. When doing the drawings, the extrusions are fairly straightforward and easy. But where I am having problems is when I draw the castings. They have different wall thicknesses, ribs, chamfers, rounds, etc. The problem is not with drawing the first piece of the frame, it is when I draw all of the succeeding parts. When I go to shell, chamfer, or round, I get into a lot of problems because the action I am trying to perform doesn't stop on just the piece I am currently constructing. For instance, a shell operation tries to shell the entire model up to that point, even though the previously constructed parts don't need it. Now I know that someone really proficient with such tasks could probably do it within a single part file. But for me, it just seemed easier to construct the model exactly as the original was constructed; one piece at a time. By starting as an assembly, then constructing each individual part within the assembly, it allowed me to more easily control the process and final shape of the individual parts. But now I am looking to bring the drawing back into a bigger assembly. Now I can bring the entire assembly into another drawing, but I am having problems with that as well. Whenever I insert an external assembly into another assembly, it works just as is should, until the next time I open the file. If I restart Pro E and try to reopen the parent assembly file, Pro E can't find any of the inserted assemblies, I have to go manually locate them one at a time. I don't understand why this is happening, because I can insert an individual part from an assembly, and it works every time the file is opened. But if I insert the entire assembly, contained in exactly the same folder, it can't find that.

[ArisTroulis]

Ok then, if you have every component of your assembly as a seperate part with all your shelling, round etc features finished you can either merge them into a new part from the assembly using component Edit --> Component operations, or you can import to a new part with external merge.

[ptc-301855]

In my opinion, you could use inheritance. You can create one part with only planes and coordinate system. Then, you use a inheritance to 'merge' each part into one. The negative point is to create the assembly again. The positive is having all dimensions in one model only.

[DELETEME]

"José Martinho Pelacani Junior" wrote:

In my opinion, you could use inheritance. You can create one part with only planes and coordinate system. Then, you use a inheritance to 'merge' each part into one. The negative point is to create the assembly again. The positive is having all dimensions in one model only.

[mnogradi]

Many thanks...it perfectly works for me.

[KrisR]

I've actually posted an "Idea" about this for PTC to evaluate. Please vote on it if you are in favor of it. Should be close to the top of the list on this page"

http://communities.ptc.com/community/creo?view=idea#/?tagSet=undefined