Assembly - Insert Plane from Part studio

james_close

While in an Assembly Studio allow inserting Part Studio Planes to compliment the current options.   This allows multiple in-context Part Studios within an Assembly reuse a single Plane definition.  Currently you must redefine common planes in each Part Studio.

lougallo

@james_close We do not allow planes in the Assembly however you can use mate connectors which can be added to the assembly origin.

james_close

Hi,  Thanks for the comment.
You allow Parts, Sketches and Surfaces defined in a Part Studio to be Inserted to an Assembly.  I am not sure why a Plane defined in a Part Studio would be a problem or architecturally different. 

I use a Top down method of modeling starting with a Part Studio.  That becomes the "template" for defining, sizing and locating the balance of a product.
The Part Studio components ( sketches at this point ) are inserted to the Assembly.   New In-Context Part Studios are then created within the Assembly and "Use" the original "arrangement" sketches entities to define the In-Context Parts.
The original Part Studio has Planes defined based on the Sketch geometry.  I currently have to recreate those Planes ( as needed) in each of the derived In-Context Parts.

Mate connectors seem to be aimed at Bottom up modeling.  I realize that the In-Context Parts are not "mated".  I have gone back to add the Mate connectors, but I am struggling to see the benefit when modeling Top Down.

Thanks, Jim 

john_mcclary

@james_close

Planes are not allowed, because there is no need. A mate connector is a plane/vertex/axis all rolled into a single powerful configurable point.
You should be asking, why doesn't other CAD do it this way 

Although it can be annoying that you cannot call upon the existing planes in a part studio, but the general idea is, you will be modeling multiple parts in the same studio. So you would only benefit from the initial part that you happen to center along the central planes. At which point you would have to add in the planes manually anyway as you would in other CAD programs.

james_close

Wow, almost real time support !

I am still not sure how Mates work in a Top Down process.  I did not need Bodies to align anything given the Top Down modeling.

I am a long time CAD user/admin and have dealt with the the historical Part/File relationships ( and limitations) of many systems.
OnShape's "Studio" concept certainly changes the game, but is not in play for this request as far as I can see.

My Document is named RollHolder and is public

Here is the initial Part Studio containing the "Arrangement" sketches and a Plane


 
Here is the Assembly that used the Arrangement sketches



Most subsequent Part Studio's are In Context based on the initial Sketches,

A series of the In-Context Parts needed the Plane HubCenterPlane

This is the first OnShape model that I tried to maintain a clean models ( no cheating) .  I was mostly successful.
There are concepts/capabilities of OnShape that I have not back fitted into the Document as yet.

Thanks,   Jim

john_mcclary

I see your point, when you have only sketches and no model to own the connector in the assembly...

Here is a work around for you. Not a single click, but it will feel more familiar to you.

Maybe you can get someone to make a featurescript for you that lets you make it instead of a plane.

Create your plane in the part studio, then add a sketch and draw a square with a label. Insert that into your assembly.

https://www.youtube.com/watch?v=xLxi_JplMHs

james_close

John,
That would be an effective solution. 
You could also sketch in local coordinate definitions to compliment the plane definition.
Thanks !

I still think Planes should be included though, just seems to be a natural capability without having to resort to adding weight to the model.

Jim

MBartlett21

@james_close
Instead of using in-context, have you tried the derived feature?
It allows you to derive planes, parts, sketches, etc from one Part Studio to another

james_close

Hi,
I did not try that originally ( mentally stuck in Solidworks mode).
I just did and found the following, more testing required on my part.

1. A Plane is an option to Derive.
2. All new features are named Derive #  . This masks the original object type, which can be resolved by adding to the name.
3. A new derived feature from a Sketch does not allow you to select entities with a Transform dialog

Thanks,
Jim