Creating slots - grooves

arends_arends

Hello, 

Pretty new to Onshape so excuse my unknowingness. I need some help with modeling so called grooves in my model and the most efficient way to do this.
Im moving from 3D CAD and Sketchup to more precise modeling with Onshape. 

I'm currently at this model:



And I need to get to this model: 

Here are some measurement views from a CAD perspective: 



Hope someone can help me out here.

Thanks in advance!

N. 

BenTaylor

There isn't a super easy way to do this, especially for a large number of lines. My suggestion:

1. Make a sketch on the same plane as your lines. Use the sketch slot feature to make slots centered on your centerline. Set the diameter to twice the depth you want.
2. Extrude-remove the slots into the part to the desired depth.
3. Fillet the inside edges with a radius equal to the depth.

The more holes and lines you have, the more labor-intensive it will be. There might be a custom feature that could do this, but I'm not familiar with any.
Here is an example with 5 holes: https://cad.onshape.com/documents/373c41515de22609937555e5/w/dc4dea711523077f334f0952/e/8da71f1ff64710f39e3d0935

bryan_lagrange

Like @BenTaylor mentioned there is no easy one click option. Unless there is a feature script out there that can do this.

My suggestion would be like Ben, make a sketch and use the slot feature but instead of extrude use the revolve remove.

Use one side of slot to revolve and the center line of the slot as an axis.


Other way would be to draw line paths and then sweep a profile to create the groove.



The sweep would allow you to make the grooves in less features than the revolve but still would take time to sketch path, create plane on path, and create sketch on that plane to sweep.

Like I mentioned before, these are the methods I would take unless there is a feature script out there that can simply the workflow.

matthew_stacy

@arends_arends , consider approaching this with the "Beams" feature script.  This is not the most elegant workflow, but may get the job done.  https://cad.onshape.com/documents/971dc4a05f7f88a44cbb3092/w/fa17c57f695a21145d1b4c13/e/93aa46a9fb6dce4dd8a4454e

In effect this allows you to create a negative of the "slotting" using a single sketch that can be boolean subtracted from the primary solid.  I used Ø10mm round bar for the beam cross section.  You can select a standard size or create your own custom profiles.

BenTaylor

There isn't a super easy way to do this, especially for a large number of lines. My suggestion:

1. Make a sketch on the same plane as your lines. Use the sketch slot feature to make slots centered on your centerline. Set the diameter to twice the depth you want.
2. Extrude-remove the slots into the part to the desired depth.
3. Fillet the inside edges with a radius equal to the depth.

The more holes and lines you have, the more labor-intensive it will be. There might be a custom feature that could do this, but I'm not familiar with any.
Here is an example with 5 holes: https://cad.onshape.com/documents/373c41515de22609937555e5/w/dc4dea711523077f334f0952/e/8da71f1ff64710f39e3d0935

bryan_lagrange

Like @BenTaylor mentioned there is no easy one click option. Unless there is a feature script out there that can do this.

My suggestion would be like Ben, make a sketch and use the slot feature but instead of extrude use the revolve remove.

Use one side of slot to revolve and the center line of the slot as an axis.


Other way would be to draw line paths and then sweep a profile to create the groove.



The sweep would allow you to make the grooves in less features than the revolve but still would take time to sketch path, create plane on path, and create sketch on that plane to sweep.

Like I mentioned before, these are the methods I would take unless there is a feature script out there that can simply the workflow.

matthew_stacy

@arends_arends , consider approaching this with the "Beams" feature script.  This is not the most elegant workflow, but may get the job done.  https://cad.onshape.com/documents/971dc4a05f7f88a44cbb3092/w/fa17c57f695a21145d1b4c13/e/93aa46a9fb6dce4dd8a4454e

In effect this allows you to create a negative of the "slotting" using a single sketch that can be boolean subtracted from the primary solid.  I used Ø10mm round bar for the beam cross section.  You can select a standard size or create your own custom profiles.

arends_arends

Thanks for all the replies! Very helpfull.
Just after posting here I created this using a less orthodox way to create the grooves:


It sort of got the job done but it needed some sketching. But the radius of the groove now excists out of 2 chamfers of 14,9 mm so its not completely rounded and probably not the best way to do this. 

I will check out the above posted methods to see what´s most efficient. All what´s left to do now is creating some sloped planes and add some text on it. 

Thanks again. 

EvanReese

I spent a little time writing a feature to do this over the long weekend since it seemed like the right amount of challenge. Give it a try!
https://cad.onshape.com/documents/607da6873450247969c4305d/w/cafaca7c9fcd3e9db77ff79b/e/d9666dc4c843633a9286bfd6

To add it, click the "+ custom features" button and click "Channel FS"

bryan_lagrange

That's awesome @Evan_Reese