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2parts into 1part

Question asked by brian kohlenberg on May 29, 2012
Latest reply on May 29, 2012 by Daen Hendrickson

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Hello colleagues,

How do I make a 2part assembly a 1assembled part, WITH NO PART LINES where the 2 parts meet, thus keeping the dynamic link to the original 2 parts so that changes to either of the original parts will update in the 1 assembled part.

Keeping the information/properties for each unique part separate is needed: Thus save as "Parasolid" or "Part" options are VOID.

Perhaps a feature improvemnt to the "advance mates" tool...a ?combine/join/seem/assemble? that would elmenate the seam/edges found on an assembly/assembled-part.

or Save as an "Assembled Part"?

i don't know,

tell me what you know,

Brian K

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David Suelflow May 29, 2012 6:31 PM
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Why does it need to be an assembly? Could you not use a multi-body part with 3 configurations? One being left side only, another the right side only and a third with them joined/combined.
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- brian kohlenberg @ David Suelflow on May 29, 2012 6:51 PM
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  David, I feel It needs to be an assembly for best results on its' drawing & each side has unique notes for the drawing too.
  when we detail this assembled part for manufacturing right now i have to hide the line on the drawing that is the joint line circled in red in the picture.
  -Bk
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  - Ryan Brumund @ brian kohlenberg on May 29, 2012 7:14 PM
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    I don't know of a way in an assembly file, but you can create an assembly of sorts in a part file. If you do a new part file you can Insert->Part... to put in your first "part". Repeat for your second "part" and position where you want it to go. After the two parts are there you can Insert->Features->Combine... to combine the two part bodies into a single body. Assuming the two diameters are the same the line should go away, the "assembled part" is using the original part files, so any updates should carry through. However, I am not sure if you can pull custom properties from the subfiles into the drawing.
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Dave Klimas May 29, 2012 7:05 PM
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Brian,

You can accomplish this by inserting one part into the other. "Insert"--->"Part". Make sure the "Break link to original part" is un-checked.

Then combine the two solid bodies. Then weld line should go away.
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- Dave Klimas @ Dave Klimas on May 29, 2012 7:07 PM
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  I guess if you wanted them totally separate insert both into a new part...
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  - Dave Klimas @ Dave Klimas on May 29, 2012 7:11 PM
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    So after reading the second paragraph again, doesn't look like that's an option.
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- brian kohlenberg @ Dave Klimas on May 29, 2012 7:35 PM
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  Dave, A part only has one set of properties, but an assembly links to all it's parts's properties.
  The weld line does go away when combined, but the information/properties form each combined part are not available on the drawing, just the one.
  Dave, those were great instructions thanks.
  -Bk
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  - Dave Klimas @ brian kohlenberg on May 29, 2012 7:52 PM
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    Yeah sorry about that...it took reading what you wrote a couple of times for it to sink in. Ha! You definitely stumped me.
    
    What if you were to revolve a surface in one part that extended over the other part to the edge of the other so it essentially "hid" the split line? No idea if that would actually work or not, but at least it shouldn't affect the mass properties.
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    - Daen Hendrickson @ Dave Klimas on May 29, 2012 9:16 PM
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      Adding to Dave's last comment, you could create this "hiding" revolve as a separate configuration in the part. You could then document each part separately if needed with the true-built configuration and put the two together in an assembly with the "hiding" configuration.
      
      Without knowing your specific requirements, could you not place your differing properties into configuration specific areas and then use the part-in-part methods. Your drawing could then point to the configuration specific data.
      
      Daen
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2parts into 1part

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