How can you make this happen?
The most practical way is to make a sketch of the centerline path of the rope and then do a sweep using a circular profile. This is simple stuff and since it looks like you are new to this forum it is reasonable to assume you are new to SolidWorks. If that is the case then I highly suggest you take full advantage of the following resources:
1. The built-in SWX tutorials
2. SWX Help
3. Frequently Asked Forum Questions
4. FAQ - Part 2
These things will dramatically shorten your learning curve and make your questions better.
If you want to model your rope showing the twists and all that detail then you are talking about something that is doable, but a bit more involved. I highly encourage you to NOT do this unless it is for a detailed view as it would be computationally intensive and unnecessary for almost all cases. Similar to modeling helical threads in an assembly, it is not necessary and a waste of effort and resources.
Can you attach your assembly here?
Are you familiar with Sweep?
Are you familiar with cosmetic appearances?
I do this all the time with hydraulically lifted frames using cylinders pulling wire rope around sheaves.
Some setup first.. My sheave/pulley parts all have construction sketches to describe the centreline of the proposed cable/wire rope, correct for the sheaves pitch. I also use construction line sketches in the sheave/pulley parts to assist position the sheaves relative to each other with mates where they are required.
Insert a New Part inside the assembly that has the sheaves/pulleys. (Best is "In-Place" mated at origin.) This will be your Cable/Wire Rope.
Now edit this part (In-Context) and simply run a 3D Sketch within your cable/wire rope part between the sheaves/pulleys and your predetermined end points, It is better to sketch directly over the construction lines and use relations like co-radial, Co-Incident, etc. ("Convert Entites" can be a bit flaky here..)
You may need to tweak a little to get proper tangent connections.
Apply a custom weldment profile for the cable/wire rope diameter and strand count, core, etc along the sketch.Remember to tick the boxes for "Merge Arc Segments" (or perhaps use "Combine" later.)
Use "Insert Part into Part" to add your eyelets, swages, clamps, etc. later within this Part.
Locate these inserted hardware items with "Locate Component with Move/Copy Feature"
(Although, I assume this can be done in an Assembly, I prefer a Multi-Body Part file.)
If done correctly, this method will also enable the Weldment Cutlist to provide you the correct length of cable required. (the primary reason I do it this way)
And it should update with refresh when any other component in the upper assembly moves.
If you mean to have a fixed length rope. Use a 2D sketch on a plane to plot your cable/wire rope path, you should be able to use the "Make Path" sketch tool on the cable sketch path and assign a preferred length. Attach the sketch path to each end you propose to connect.
This should enable movement at one end of the wire rope to effect displacement at the other. Usually not until after refresh. I do this less frequently.
(It's a pity we don't have the "Make Path" option for 3D Sketches..!)
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