Derived Component Feature / Body As A Work Surface?

john_hammons643

Hello! I'm new to Onshape and was wondering if Onshape has the feature that allows deriving a "body as a work surface" from a derived component similar to how Autodesk Inventor does it? Any tutorial or link that offers instruction on how to use this feature (if it exists) would be helpful!

Thank you! 

NeilCooke

You mean the Derived feature?
https://cad.onshape.com/help/Content/derived.htm?Highlight=derived

john_hammons643

I'm trying to prepare for a high school boat design competition and we have used Autodesk Inventor in the past. However, that will not work this year because we are beginning the school year 100% virtual and my students have Chromebooks which will not support Inventor. I am hoping the Onshape platform will be able to do what we need. As I work through some of the process, I would like to post my problems in this thread hoping someone can lend a hand.   

john_hammons643

First off, we need to be able to see the mass properties....specifically all centers of gravity and also all the moments of inertia.  You'll see in this pic they do not appear when I select the mass properties button. How do I get them to show up? The "BargeExample" file is in the public domain should anyone need to see it.

NeilCooke

Have you added a material? Right click the part and assign a material. 

john_hammons643

I also need to be able to use the "Derived" command to create a "Body as a Work Surface." Is that possible with Onshape? I see how to use the "Derived" command but I do not see the "Body as a Work Surface" option in Onshape like what is available in Inventor.

 

steve_shubin

@john_hammons643

I’ve never used Inventor. I’m curious about that term ‘Body as a Work Surface’. Could you explain what ‘body as a work surface’ is or what it does or how it works

john_hammons643

OK....so I watched a couple youtube vids....looks like there is no "Body as a Work Surface" feature in Onshape like there is in Inventor. In the meantime, I have derived a master sketch which I then used the surface modeling technique to give me the side of the barge in the pic. I still need to be able to get the mass properties to work. Anyone have any suggestions? Thanks!

tim_hess427

@john_hammons643 - I think the mass properties question is answered in a previous response and my have gotten buried under other replies. For the mass properties to work, a material needs to be assigned to the part, first. You can right-click on the part in the list, and select "assign material". 

I'm also not sure exactly what "Body as a work surface" is supposed to do. If you could describe how its used, I'm guessing there is an alternative workflow that can accomplish something similar. It looks like you've been able to derive things. Something else worth looking into is "in-context design". That allows you to create an assembly, then create a new part studio where you can design parts that reference the assembly. 

NeilCooke

If you derive a solid into a part studio it will be a a solid. If it has no material it will not be included in any mass properties (I assume that is why you want a surface). If you really want a surface, you can create a zero Offset Surface of the faces you want then use Delete Part to delete the solid. Alternatively create a zero Offset Surface in the Part Studio you’re deriving from and derive just the surface. 

In-context design as suggested by @tim_hess427 is also valid - with that you can reference any face from an assembly. 

john_hammons643

tim_hess427 said:

@john_hammons643 - I think the mass properties question is answered in a previous response and my have gotten buried under other replies. For the mass properties to work, a material needs to be assigned to the part, first. You can right-click on the part in the list, and select "assign material". 

I'm also not sure exactly what "Body as a work surface" is supposed to do. If you could describe how its used, I'm guessing there is an alternative workflow that can accomplish something similar. It looks like you've been able to derive things. Something else worth looking into is "in-context design". That allows you to create an assembly, then create a new part studio where you can design parts that reference the assembly. 

It's probably easier to show you than to explain....here is a video explaining how to find the centers of gravity of a plate on a boat design....I used the "Derived Component command in Inventor along with it's "Body as a Work Surface." Please watch the 3:15-4:00 minute mark of this video:

https://www.youtube.com/watch?v=xSDHWuIJ7xw&t=2s  

john_hammons643

steve_shubin said:

@john_hammons643

I’ve never used Inventor. I’m curious about that term ‘Body as a Work Surface’. Could you explain what ‘body as a work surface’ is or what it does or how it works

See post 6 please....thanks!

NeilCooke

@john_hammons643 - are my posts not showing up in your feed ?    There is no equivalent in Onshape. You can leave the Derived part as a solid or you can convert it to a surface using the techniques I mention above. 

tim_hess427

@john_hammons643 - Thanks for the video link. If you're trying to do the same thing on Onshape (calculate mass properties for individual panels), then, I think @NeilCooke's suggestions are the way to go.

You could work in the same part studio as the original boat, or derive the whole boat into a new part studio. Then, you can select individual faces, use "thicken" to get a new body for a single panel, apply a material to the new panel, and then you can view the mass properties for that single panel. 

If you really the individual surfaces as an intermediate step, you can select a face, use the "offset surface" tool to create a new surface, but just set the offset distance to zero. Then you have a new surface coincident with the model that you can thicken/manipulate just like in your video. 

john_hammons643

@NeilCooke and @tim_hess427 thank you!! Yes. I have read your posts and what you suggests looks good! I will get going with this soon! There is more to this competition and will post questions as they come up but this looks like a great start! 

john_hammons643

I was successful...looks like your gif above really helped out @NeilCooke

Now comes the fun (sarc) part of the competition....using Simpson's Rule!