Creating a curved channel fixed to side of tubular piece

I’m trying to create a channel affixed to the side of a tubular section to be able to insert a cable or rod which can be moved back and forth within the channel. I thought revolve or loft would do it but it didn’t seem to work. Any thoughts? The channel and tubular piece would be all one part. Attached are a couple images. The blue line represents the proposed channel. It was hand drawn so it may be a little crooked but as you can see it starts at the top of the tube (12 o’clock) and wraps around the side along the length of the tube and ends at the underside of the tube (6 o’clock). The shape of the exterior of the channel can be rounded or just about any shape but must be hollow on the inside to allow for the insertion of the cable or rod. The cable or rod would be about 2.5millimeters or so in diameter and about 14 inches (355 millimeters) or so long.

Project a sketch on the cylinder and sweep a profile on it.

How do you project a sketch on the cylinder that curves around the circumference? Incidentally, I’ve tried that with splines but I can only seem to get the splines to stay on one plane.

Just use the project tool, from the tools menu.

https://support.shapr3d.com/hc/en-us/articles/360012231934-Project?mobile_site=true

Thanks for the suggestion but I can’t see how this would work on my example. In my case the channel needs to wrap around the cylinder.

@Benjb Something like this:

That’s close but the beginning and end of the line curve perpendicular to the length of the cylinder whereas they need to be parallel to the length. The goal is to be able to pull a lever that moves parallel to the length of the cylinder which puts tension on the cable or rod within the channel (or cable) housing. Thanks though. Was this done with project?

@Benjb In the ScreenShots, I am attempting to show you the results of using Project.
The best thing to do is take the advice given by @Istvan_CEO_Shapr3D.
Use your Design and use the Project tool to place a line on your ‘Tubular’ Objects surface.
Draw the Line on one of the main Planes or Add a Construction Plane [CP] and use that.
I used the CP because it looks like a sheet of ‘see through’ Tracing Paper and can be moved around as needed.
Follow the On-Screen directions to Project the Line from the CP/Main Plane onto the surface of your ‘Tubular’ object.
Directions appear in the Central Side Menu and the Centre Top display.
First and foremost you need to succeed in placing a Projected Line on an Object or Surface.
When you make this happen you will begin to realise the magic of S3D.

If you want the line to start and finish 180º apart at opposite ends of the Object you will have to angle the line appropriately and make sure it is long enough. Don’t worry about exact length an surplus will be discarded.

If your attempts leave you disappointed ask for help on the point giving you problems.
Like the man said ‘Need help? We are here.’

Benjb

Is this what you are trying to achieve?

-Mike

The path of the channel looks like what I’m trying to do, however I’m looking to have something that sits on the exterior of the cylinder so there’s not a groove like what you have. But that looks really good. Did you do that With project also?

I did a quick project just now but still didn’t get the result I needed. I’m going to try again and see if I can improve it by making adjustments to the path. Thank you and I will let you know how it goes.

Hi there,

I used Revolve to create the channel, Revolve to create the cylinder and did a Union. This is quick and dirty as I didn’t clean up the ends.

-Mike

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The curve of the channel is pretty spot on. Is it possible to create it with another profile besides the square/rectangular shape it has? I guess I have to learn the ins and outs of revolve because I can’t see how you created the channel using that. Thanks again!

Here I created an odd looking profile of a channel just for discussion sake. This video just steps forward with a bunch of Redo’s. Here are the steps-
Sketched profile(s)
Revolved channel just to show what it look like in 360° then deleted as it is not needed
Revolved channel with a distance of -8 and at 200°
Hide revolved channel and create 2 cylinders. The left one is used later for Subtract
Show channel and Union with cylinder.
Subtract from the left end just so you can see the relationship of the initial profile next to cylinder with attached channel.
Let me know if any questions.

Regards, Mike

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Wow thanks, I’m not sure it will work but I’m going to try and see if I can get it to do what I need. I’m new to S3D so I had to read your steps about 6 times. After grasping them I now think they were excellent directions.
I’m attaching another pic with a sample profile for the channel I need. Yours is open but it looks like I should be able to revolve a closed channel that can enclose a cable. The red square in my pic is a sliding button/lever that is to pull back on the cable which will pull back on a lever at the other end of the cylinder.
The main thing I’m dubious about with your method is that the beginning and end of the channel need to be parallel to the length of the cylinder for about and inch or so to be in line with the sliding lever/button and lever at the end. Also the channel should probably have as smooth a curvature as possible so that the cable slides through without resistance.
Thanks again!
Benj

Here is another version. Is this what you want to achieve?
I made the channel semi-transparent with a red wire or cable running through it.

-Mike

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That’s it! Was that done with revolve? Same numbers -8 and 200? I still have not been able to get the free time to replicate what you’ve done on my own but hopefully today. I still need to figure out how to get those ends to be parallel.
Thanks,
Benj

Hi there,
I used Revolve to create the helix path of the channel and then used Sweep to create the body. I will elaborate further later today with a video showing my steps.

-Mike

I sketched the profile of the cylinder and external channel with hole as one face.
In a plane 90° to the cylinder, I sketched a dummy triangle face just for the purpose of creating the helical path for the channel. Note: the tip of the triangle is at the center of the channel profile.
Create the body of the helical triangle using Revolve then temporarily hide it. Hide the triangle sketch and show the cylinder sketch. Now use Sweep- select the face, then Next, then show the helical triangle and select the top (tip) of the triangle. This edge becomes the path for the sweep. Done!
I hope this helps. (I made a YouTube video as the file size was too big to upload.)
Regards, Mike

This looks like it works. I’m still trying to process the steps, mostly the why on some of the steps. I don’t get the triangle yet. The directions are explained nicely I’m just just new to S3D since I’ve just switched over from the free version of SketchUp.

It looks like after I figure this out then I just need to extrude the ends of the cylinder to make room for the sliding button and lever.

I wish I could try this myself more quickly but work is making that difficult right now and since basic skills like lining up the triangle to the center of the hole are things I still have to learn, I’m not able to get back to you as quickly as I’d like. I do truly appreciate all of your help so far.

I’ll post my results as soon as I can.
Thanks again!
Benj

There are a variety of ways to achieve what I created for you. I needed a curved edge in order to get the helical path of your channel. There may be other ways to obtain that edge, but what I did worked for me. To make that edge I used the top tip of the triangle. Again, the triangle was only used to make the curved path, then it was discarded.

To line things up you can draw a horizontal line on one plane and offset a line, say 3". Go to a plane 90° from the first one and draw and offset 3". There are other ways to do this. You can draw the triangle and channel circle on one plane then use Transform- Move/Rotate/Scale to rotate the sketch of either the circle or the triangle.

When it’s time to use Sweep, you can use only the profile of the channel. Then extrude a cylinder as a separate body. Now you can create your desired distances of the edge of the channel relative to the cylinder.

There may be other or easier steps to use than the ones I used. Again, the method I used is what worked for me given my limited knowledge of this great app.

-Mike