Connecting two bodies with a spline 2

[Waidesworld]

I am making a box where a wire coming from the top side will connect to a copper bar within the box. The attached jpeg shows the box and I added two red lines to show what I want to see happen.

I was trying a 3D spline but not having much success.

drawn to design, designed to draw

 

[Eltron]

What do you mean by not having much success? When I do 3D splines for wiring or plumbing I've found it helps to split the screen into 4 views.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[TheTick]

Try using construction lines to anchor the ends of the spline. Put line endpoints where the spline endpoints and make lines normal to the surface the spline connects to. Constrian the spline ends tangent to the construction lines.

You may also want to draw some points or construction lines at key junctions to anchor your spline.

 

[Waidesworld]

I can draw the splines between the parts but I can't for the life of me see an option to sweep....

drawn to design, designed to draw

 

[Eltron]

Did you draw your profile (small circle) for each spline, and is each spline in a separate sketch?

Dan

http://www.eltronresearch.com

Dan's Blog

 

[CorBlimeyLimey]

Did you create the splines in a 3D sketch in the assy, or in a new part?
An extruded-sweep can only be created in a part. Material cannot be added in an assy.

 

[msquared48]

Your title caught my attention...

Mike McCann
MMC Engineering

 

[NomLaser]

Since you left it so vague as to why it's not working I'll try and give you a couple of things to check.

Did you create a profile sketch for it to sweep
Make sure that the profile is normal to your 3-D sketch
Make sure that profile sketch is in the part file
Check to be sure that the 3-D sketch tangent to the wire
The 3-D sketch needs to be one spline

What I have found that works best is to create an empty part file. Insert it into the model and mate it via planes to the assembly origin. Edit the part in-context and create a 3-D sketch with line for the starting point and the end point. Make those lines concentric (or lock them in place somehow) to the existing components. Create a line between the two then add sketch fillets to make it curved. Exit the sketch and go back to the part and add a plane normal to the sketch and add a profile on that plane. Sweep and you are done.

If I wanted to make it with a spline you just use a spline instead of a straight line between the start and end lines.

This has been the easiest way that I have found to make wire without using the routing software.

 

[ArtemTat]

Make also sure you aren't in the Edit Sketch Mode. in this case the Sweep command is suppressed.

Artem Taturevich, CSWP
Software and Design Engineer
AMCBridge LLC

http://www.amcbridge.com

 

[Waidesworld]

Thanks CorBlimey, that's the issue. I was in assembly and wanted to add into it. I will add them to one of the parts and then see where I end up. I don't get to draw every day which is why my answers are sporadic.

drawn to design, designed to draw