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Combining two bodies to make one..

Question asked by Jared Morisset on Apr 16, 2013
Latest reply on Apr 17, 2013 by Jared Morisset

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I have two plastic parts and they are actually designed to fit together in an assembly, but now they want to get it quoted as one part. So what i have been doing is bringing in one of the two parts into a new part, then bringing in the other part using>Insert>part and selecting my part. Finally where i am getting stuck is trying to COMBINE the two parts and merge as one...

I would have just simply re-modeled it to make everything cleaner, but it is a very intricate part with multiple contoure and other such features. I even tried to extrude between the two but keep getting the invalid geometry/zero thickness message..

Any suggestions??!

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Patrick O'Hern Apr 16, 2013 2:40 PM
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Try adding a small amount of extra material to the upper body so that the two have interferance. This should help with the zero thickness error.

If that doesn't work, can you post the file?
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- Jared Morisset @ Patrick O'Hern on Apr 16, 2013 2:45 PM
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  I work for an R&D company so i dont think they would like it if i post the file.. however I did post a fraction of it with the snip-it tool and attached it to the original question
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Philip Lewis Apr 16, 2013 2:48 PM
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Instead of starting a new part try starting with a new assembly. Put the 2 parts together and then save the assembly as a part. That might help the combine.
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Alin Vargatu Apr 16, 2013 3:10 PM
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What about grouping them in a sub-assembly? That will give you the 1 part number component in the main assembly.

Otherwise, please post the files here and we will troubleshoot the zero thickness problem.
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Jason Swackhamer Apr 17, 2013 9:33 AM
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Jared-

Two additional suggestions if you haven't tried them:

1. Run an entity check on both bodies. If there's a "bad face" or "general fault", these will have to be fixed before combining.

2. Sometimes when we run into a problem like this, we'll split the bodies in half and try combining one section at a time. If one section combines, then delete that body and divide the ones left over in half and apply the same proceedure. This can help to narrow down precisely where the problem is occuring.

Hope this helps,

-Jason S.
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- Jared Morisset @ Jason Swackhamer on Apr 17, 2013 9:36 AM
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  How do yu run an entity check? Also, after check has been ran.. what would be the best way to fix?
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  - Jason Swackhamer @ Jared Morisset on Apr 17, 2013 10:43 AM
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    Jared-
    
    Under the "Tools" menu, select "Check...". A dialog box will come up. Select the radio button for all, and check the "Stringent solid/surface check" checkbox.
    
    Run the check. If there are errors, you can select the item in the "Result list", and it will highlight on the model. This even works with the "General Fault" error. Sometimes you can spot a face error, because the face shows as transparent.
    
    How to fix? Not so simple...let's see if you have any errors before diving into that.
    
    -Jason S.
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    - Jared Morisset @ Jason Swackhamer on Apr 17, 2013 10:55 AM
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      i ran the check and got no invalid edges/faces found..
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Lenny Bucholz Apr 17, 2013 9:49 AM

there a couple ways to try this if the combine doesn't work.

put the 2 parts in an assembly and insert a new part in the assembly then use the old old tool called join, was there before multible bodies and it will try to force the 2 parts together to make 1 part....old way we made weldments..back in the day.

or you may have to use surfacing, deleteing faces and extendind triming filling.... and then knitting back to a solid.

if you cannot get, talk to the powers that be and explain there are people willing to help make this happen to help get the file to work.

I have signed many none discloser as many others have... just an email sign and fax.

one last way is to add material to one part so that the intersect.... but I'm thinking surfaces. or you just have to rebuild as one

Creating a Joined Part

In an assembly, you can join two or more parts to create a new part. The join operation removes surfaces that intrude into each other's space, and merges the part bodies into a single solid volume.

To join parts:

Create the parts that you want to join, then create an assembly containing the parts. Position the parts as desired in the assembly. The parts may either touch each other or intrude into one another.	$art\jn1_shg.gif$
Save the assembly but do not close the window. Insert a new part into the assembly: Click New Part on the Assembly toolbar, or click Insert, Component, New Part. Click a plane or planar face on a component. In the new part, a sketch opens on the selected plane.	$art\jn2_shg.gif$
Close the sketch. Because you are creating a joined part, you do not need the sketch. In the FeatureManager design tree, right-click the new part name, select Rename Part, and rename the new part. Click Insert, Features, Join. Make selections and set options in the Join PropertyManager. Click to create the joined part.

$art\jn3_shg.gif$	$art\jn4_shg.gif$
Before join - coincident faces	After Join - faces are removed

To return to editing the assembly, right-click the assembly name in the FeatureManager design tree, or right-click anywhere in the graphics area, and select Edit Assembly:<assembly_name>, or click Edit Component on the Assembly toolbar.

The joined part is fully associative to the original parts and to the assembly. Any changes made to the original parts are reflected in the joined part. If the parts move relative to each other in the assembly, the joined part changes also.

Search 'Creating a Joined Part' in the SolidWorks Knowledge Base.

Message was edited by: Lenny Bucholz

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Jared Morisset @ Lenny Bucholz on Apr 17, 2013 9:49 AM
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Oh my garsh, i gotta learn surfacing!! Does SW offer tutorials on surfacing??
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- Lenny Bucholz @ Jared Morisset on Apr 17, 2013 9:58 AM
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  Jared Morisset wrote:
  
  Oh my garsh, i gotta learn surfacing!! Does SW offer tutorials on surfacing??
  or join or alot of other things to make it work.
  
  have you tried move face? just thought about that... top piece move the faces that touch the bottom and then try combine??? never know
  
  Message was edited by: Lenny Bucholz
  
  Move Face PropertyManager
  You can offset, translate, and rotate faces and features directly on solid or surface models.
  Click Move Face (Mold Tools or Features toolbar) or Insert, Face, Move. You can also right-click a face and click Move Face, or select Move Face on the Direct Editing CommandManager tab.
  In the PropertyManager, set the following options, then click OK .
  Move Face
  Select one of the following:
  Offset . Offsets selected faces or features by a specified distance.
  Translate . Translates selected faces or features by a specified distance in a selected direction. Example of creating translated Move Face features.
  Rotate . Rotates selected faces or features a specified angle about a selected axis. Example of creating rotated Move Face features.
  Instant3D functionality supports editing of Move Face features. Click the Move Face feature or face and use the Instant3D arrow, dimension manipulator, or triad to edit the Move Face feature.
  Face(s) to move . Lists the faces or features you select. Use the Select Connected Faces pop-up toolbar to help you select various faces.
  Copy. Copies faces and features using the Translate and Rotate commands. You can use Instant3D functionality, such as the triad and rulers, to position and edit the Move Face features. This option is useful when you modify imported geometry. You cannot create disjoint bodies using this option.
  Parameters
  Distance . For Offset and Translate, set the distance to move the faces or features.
  Draft Angle . For Rotate, set the angle to rotate the faces or features.
  Flip direction. Switches the direction that the face moves.
  Direction reference . For Translate, select a plane, planar face, linear edge, or reference axis to specify the direction to move faces or features.
  Axis reference . For Rotate, select a linear edge or reference axis to specify the axis of rotation for faces or features.
  Search 'Move Face PropertyManager' in the SolidWorks Knowledge Base.
  
  Message was edited by: Lenny Bucholz
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- Patrick O'Hern @ Jared Morisset on Apr 17, 2013 9:58 AM
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  Yes, they do. Look in the Help Section under SolidWorks Tutorials. Select Basic Techniques, then Surfaces.
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  - Jared Morisset @ Patrick O'Hern on Apr 17, 2013 10:09 AM
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    Awesome thanks! I'm going to check it out right now..
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Combining two bodies to make one..

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Creating a Joined Part

Move Face PropertyManager

Move Face

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