Giving an part a quantity with attributes

[RonalddeBruijn]

Some parts like bolts exist in high quantities in assemblies. We want to assign quantities with attributes to parts just like autocad does, which give better performance and reduce labour. An attribute has information of quantities of a part and in this way gives the quantities to the part list. Is there an existing program to handle this.

 

[ShaggyPE]

You can add a custom property to the part file titled quantity. In this field you could put in the number of instances this part is used in the assembly you are putting it in.

The problem with this is that it is somewhat counter productive for the Solidworks environment. If you wanted to put this same screw into another assembly, the quantity would be all screwed up. You would have to create a copy of the part, give it a new name, and change its quantity property.

The way Solidworks is designed to work is to actually have the correct quantity of screws in your assembly. Soliworks will automatically generate a BOM, counting the instances of the part. I understand your reluctance to insert every screw into your assembly, but it truly is the cleanest way.

 

[MElam]

One way I have seen this done if you do not want to show every fastener:

Insert 1 fastener. Locate correctly if you wnt to balloon it on the drawing.
Create a component pattern of the fastener with the required qty. and HIDE (not suppress)the pattern.

This will give the qty count in the BOM

 

[CorBlimeyLimey]

You could also insert "empty" parts (no solids or sketches) but which have the necessary custom properties. You can still use the Origins & Planes to mate them in the correct place if necessary. That way you get the correct quantity, part no, description, etc, without the file size penalty.

from (the City of) Barrie, Ontario.

What happens if you get scared half to death twice?

 

[Standing]

RonalddeBruijn,
If you are just looking for a quick way to put a lot of bolts into an assembly without putting them at each location, you can do it like this. Create an assembly called “Bolt ½-13 x 3” In this assembly put, lets say 300 bolts. You will only have to do this once. I put each bolt at zero, mated to the planes of the first bolt within this assembly. That way if you want to move bolt 1, all will move with it. This will look like you only have one bolt in the assembly. In the model tree you will have 300 bolts. Now take this assembly and insert it into your assembly that you want 198 bolts. Place the assembly in the location that will look good with a balloon. Dissolve Sub-assembly and delete bolts 199 through 300.
Save “Bolt ½-13 x 3” at a location everyone can use.
Good luck.


Bradley