sketch vs part best practices?

jeff_mcaffer

I'm playing around with doing a house design using onshape and wonder if I'm doing it right. One example is the "studs" in a wall design. Some of the walls have sloped ceilings so the studs are incrementally taller as you go along the wall. I had assumed that I should be making "stud" parts and then assembling them into a wall. But computing the length and cut angle of each and producing individual parts to track and assemble is challenging. Effectively I'd love to have the constraints of sketches but at assembly time. Mate connectors are great but AFAICT they cannot affect the parts being assembled (e.g., stretching a part to fit between two connections).

Alternatively, I could lay out each wall in sketches but it seems like all the headers, footers and studs get joined into one part -- effectively the distinction between the "parts" is lost.

I completely get that onshape is not intended as an architecture tool but these same topics have come up for me in a few different scenarios making me question my mental model of the best way to use onshape. Pointers or insights?

Jeff

MichaelPascoe

Welcome to Onshape Jeff! 

We will get you set. There are many different approaches to something like this. Depending on your needs, some approaches will be better than others. What is your end goal? Drawings? Cutlist? BOM?

Please share a link do your document or an example picture of what you would like to do. This will help us help you better.

mahir

@jeff_mcaffer some tips.

1. When creating extrudes and other features, you can choose New instead of Add. This will make a new part instead of joining it to existing geometry.
2. There's nothing wrong with using the part studio as your assembly and placing every part you need there. This tends to take care of the issue of relating individual parts to overall constraints (e.g. studs meeting a roof line). If you do end up using an assembly, at the very least each unique part (or length stud) should be modeled in the part studio. These unique parts can can then be patterned in the assembly.
3. Another approach is to use configured parts - like a stud that lets you dial in the length for each instance. This would let you take a Lego approach and assemble the house stud by stud. I wouldn't suggest this since it would get tedious. However, it's a valid option and can come in handy when used with other methods.
4. Yet another option is in context part studios. These let you modify parts based on their assembly context.

I know you probably don't know how to actually implement most of these ideas yet, but it's a start just to get the gears turning.

matthew_stacy

@jeff_mcaffer, this application practically begs for the Onshape "Beams" tool.  There is an excellent tutorial in the Learning Center.  I believe that you will have to create your own custom profiles for dimensional lumber.

The beauty of this approach is that you can layout the framing for an entire wall in a 2d sketch (or series of 2d sketches) and let Onshape do the heavy lifting and repetitive task of instantiating parts.  Here's a quick example:

steve_shubin

I really like the way @matthew_stacy has shown with FRAME
I need to spend more time with that tool and probably should watch that video
Almost got everything the way I wanted except for one stud
Thanks for showing that Matthew

Here are a couple of GIFs showing an additional way

https://cad.onshape.com/documents/eb9554d2c6360b045262dee1/w/fb14a496fdae4d929c23c279/e/8d511e3df200bc7d82ab5122

eric_pesty

The frame tool should really be the best way to do this, it's meant for it (and you can still do some modifications to any frame member, like move/replace face or body transforms before generating the cutlist)!

However here's another potentially useful technique:
If you create the stud by extruding from the bottom and set the end to condition to "up to face" to the top of the frame. If you then pattern the feature (not the part!) and select "apply per instance" it will make every instance in the pattern go up to the face.

I would also recommend using the excellent "linear pattern+" custom feature to avoid having to manually figure the number of instances in patterns.

Here's an example:
https://cad.onshape.com/documents/23467be153109d902a35ab43/w/af0feb4d7ff8f44dd40323df/e/56cfe37697c7434a8882870d

Also note the use of "move face" with the "translate option" to move the end stud back without having to manually adjust the length!

jeff_mcaffer

Wow. Thanks all for the suggestions. It'll take me a bit to digest the different approaches but it all certainly looks promising (and I can tell I've been working with rocks and sticks so far). I quite like the idea of doing as much as possible in sketches where you have constraints and all the other good bits. But I also like the composability of assemblies. Linear patterns as shown here will help with a lot of this. I hadn't discovered those yet.

I'm sure I'll have more questions, but this has got me pointed. Thanks again.

Jeff

steve_shubin

@jeff_mcaffer

A decent program like Onshape will do a lot of the figuring for you

If you’re talking about rake walls, you’re likely talking about following the roof line

Framers talk about roofs as rise over run

Onshape has a lot of formulas built into it. And if I input the roof slope into one of the formulas, it’ll automatically figure the degrees for me.

So if I input a 4 in 12 (meaning 4 inches of rise in 12 inches of run) into the inverse tangent formula, we’ll here is what I get