If you have to assemble many clamps to your base plate, or if you have some custom parts to be bolted or riveted into place in your SOLIDWORKS assembly, then this SOLIDWORKS Smart Components article is for you.
In SOLIDWORKS you can make your part files act smart upon inserting them into your assembly files. You can make smart components to carry bolts, rivets, or any custom components with them when you assemble them to your top level assembly file. In addition, instead of creating bolt holes in the assembly environment to use the inserted component as reference, you can get smart components to carry over their required holes into assembled component. In this article we will walk you through making smart components.
Make SOLIDWORKS Smart Components
In this article, a case study is demonstrated to show the necessary steps. However, it can be easily expanded for your particular applications as well. The case study is we need to insert a clamp into an assembly and mate it to a plate. We need to bring in bolts and also bolt holes on the plate along with the clamp model.
- Create plate model and then insert it into a new assembly as the first component for the assembly.
- Insert clamp into that assembly and mate bottom face of the clamp to the top face of the plate.
- Use “Edit Component” command to edit the plate within assembly. Add two Hole Wizards to the plate using the clamps bolt holes as reference.
Note: Cut extruded holes will not work for Smart Component command and will not insert into assembly later on.
- Insert bolts from SOLIDWORKS Toolbox. The toolbox items will snap in place upon dragging if the mouse is pointed to the clamp’s bolt holes.
- Now we need to make the clamp a smart component. Use Menu Tools > Make Smart Component
- Select the clamp under Smart Component, the two bolts under Components, and the hole wizard feature under Features. This specifies which components and which feature will be inserted with clamp upon inserting it into an assembly file.
- Check the Feature Tree in the clamp part model. There will be a Smart Feature folder on top of the Feature Tree. Expand the folder and check sub-folders to make sure of correct features, components, and references.
- Now create a new assembly file and insert a sheet metal or a plate into it. Then, insert the clamp into the assembly and mate it to the plate using coincident mate.
- Check the clamp model name in the Feature Tree. There is a star on the component symbol. Also, upon selecting it on the Feature Tree, a star symbol appears on the clamp on the graphics area. Either click on that star in the graphics area or right-click on the clamp model’s name in the Feature Tree and select “Insert Smart Features”.
- Select the top face of the plate as the smart component reference and then bolts and the hole wizard will show up on the clamp.
- Bolts and the hole wizard will move with clamp in case the clamp is moved to a different location on the plate. After moving the clamp, you need to rebuilt the assembly model by pressing Ctrl+B or selecting the rebuilt button on the toolbar.
Note: Mate References can also be used to eliminate the mating step for the clamp to the plate upon inserting the clamp into the assembly.
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