Best Way to draw a wire connecting two assembled components

[heritagesurf7]

Hey, This is my first time on the forum and I'm hoping someone here can help me out. I'm using SW '05. I was wondering if anyone knew the best way to connect two assembled components.

The issues I have run into are:
Assembly files don't let you draw circles
Assembly files don't let you sweep, only cuts

What I have done:
Creates start/endpoints for all of the wires (flat, circular faces)
Created a reference plane connecting the two components, spline a "wire", copy the spline into a new part file, sweep, import into assembly. However, it doesn't ever line up perfectly from start to endpoints.

Is there a way to construct a wire within the assembly?

 

[MadMango]

Yes, look in Help for In-Context modeling. You'll probably want to create a Combined Curve as a sweep path for your wire.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[MadMango]

Combined Curve = Projected Curve, sorry.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[SnowCrash]

I do this for cosmetics only. I create one stub of the wire at each end using a profile and a straight line path with points established on the attached part I am connecting. Then I connect them with a 3D curve made of straight sections. These curves tend to automatically align, so it is tedious. Once the wire looks decent I radius the bends with the sketch radius tool. I usually exclude this part from the BOM.
This works even if the parts you attach to move around.

--
Hardie "Crashj" Johnson
SW 2010 SP 2.1
HP Pavillion Elite HPE

 

[heritagesurf7]

Thank you both, I think I am going to try SnowCrash's first, because it seems more familiar. That sounds really similar to what I am currently doing, but can you clarify the "straight line bath with points established on the attached part"? Does that mean you just make a straight line connecting your two stubs? Then, how do you sweep your path? In assembly mode it won't let me draw circles as my base geometry and won't let me sweep.

 

[heritagesurf7]

Just for kicks I uploaded an image of what I'm currently doing. It was my mistake, I can draw a circle. However, I still cannot sweep (grayed out)

 

[CorBlimeyLimey]

You will have to create a new part and insert it into the assy, and then edit the part inside the assy.

 

[Updraft]

In assembly mode you can cut on the parts, but you cannot add material to them.

As CBL said you'll need to bring in a part and perhaps edit it in the context of the assembly.

- - -Updraft

 

[ctopher]

I agree with others here.
Each wire is a separate part that is edited within the assy.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[CorBlimeyLimey]

If creating a multi-wire harness, each wire could be a non-merged body in a multi-body part.

 

[steinmini]

I did something like that, cables for brakes and gear shifters (in SW2010, though) and started with inserting new part into the assembly, draw the lines & splines to create the path, and used the custom template I created earlier in a new folder where the other structural member templates are (eg. SW/data/weldment profiles/custom) and created the cable housing as if it was a structural member. Of course, for presentation purposes only. Found that to be a fine and easy to do way on complex routing paths. Tried that with creating wires from a transformer to rectifier and from rectifier to filtering PCB in an amplifier design, worked well. To create the template just draw a 2D circle (or required shape) and save as *.sldlfp file