Base Part in Wildfire

[michaelpaul]

I've been away from Pro/E for some time but am now working with it again. I last worked on 2000i and since then have been using SolidWorks exclusively.

Since I'm new again, the answer may be obvious but I can't find it anywhere I've searched.

I have to design plastic parts that typcially have a front and back, top and bottom, or left and right. each part is a seperate molded part but they must fit together as if they were one.

In SolidWorks, I would design the main shape of the finished part as one part. I would put all detail on this part including any fillets, draft, etc. most importantly, I would put the parting line on this part and split the draft at the parting line. I would even put the shell on this base part. basically, anything that you wanted on the fnial part that you could think of that would dictate the shape would go on this part.

then, I would create a new part and simply insert the base part into my new part as my first feature. then I could just cut the top or bottom half away at the parting line to work on the individual parts. the beauty of this is that any change you ever made to the overall shape of the part could be made to the base part adn then the two "children" parts would get updated instantly. The shapes always followed.

Can this be done in Pro/E Wildfire 2.0? right now, everybody at my work just creates seperate front and back parts and they match the dimensions manually. if anythign changes, they have to change two or more parts every time. it doesn't seem very efficient.

Thanks for the help

Michael

 

[bp]

I'm not sure, 'cause don't work with it,but I think that mold design can help you.


bp

 

[robertib]

Another option is to use a skeleton (Advanced Assembly eXtension) - the skeleton is what you would design as the main shape. Then other users would use the skeleton in the assembly to create their individual components.


I hope this helps, but Ican't give you more detail than that, since I don't have AAX.

 

[[-Skint-]]

Hi Michealpaul, welcome to the forum.


When you say "" Can this be done in Pro/E Wildfire 2.0? right now, everybody at my work just creates seperate front and back parts and they match the dimensions manually. if anythign changes, they have to change two or more parts every time. it doesn't seem very efficient ""


The only thing I can mention is that, instead of manually checking dimensions on two seperate parts, you insert the first part into an assembly and create the second part " over the top of it ". There is an option to " create part in assembly "


Hope that helps.

 

[megaladon]

another option would be to family table this


create the outer shell of it then create a cut in the middle

 

[dr_gallup]

You can do the exact same procedure in Pro/E. There are several different ways to do it, some will require the Advanced Assembly Extension. You can make an assembly of your whole part and your split part with no geometry and then merge the whole part into the split part then cut away what you don't want in the split part. That is the old school way. You can also use skeletons as mentioned previously or you can do Insert/Shared data/Copy Geometry or Inheritance from other model. Both of these require AAX.

 

[michaelpaul]

Thanks for all the replies.

in working with a colleague at work, we came up wtih what we think is the most efficient implementation of this.

we created the base part. we then created an assembly and inserted that base part using default conditions.

then, we just inserted a blank component and assembled it to the default as well. we activated the new part and then did an <insert> <shared data> <merge>. we brought in all hte datum curves and planes.

after that, we could edit and change the new part by cutting out the unnecessary sections from the base part. we did this for three parts (a front, a back, and an access door). all parts are seperate but all I need to do is change the base part dimensions if I ever want to change the overall size or shape of the part. all three "children" parts now follow.

Michael