"Group" while in Parts Studio?

christopher_owens

Hello! I have a Pattern of a part (35 instances) in Part Studio that I wanted to make a Group. I read that I have to put all the copies in an Assembly and then create the Group? Seems it would be more efficient to have the option to create the Group where the Pattern was created.

ps There is no 'Group' in "Tags"

christopher_owens

OK... so I went to the Assembly and started selecting Part 1, Part 3, Part 4...(there is no Part 1-SHIFT-Part 36) to select all at once! Good thing there is a Part 33<2> when I lost my place trying SHIFT and CTRL in the list! Once ALL the parts were in the Assembly then I could do a Part 1-SHIFT-Part 36 to select all and apply a "Fix". Now I can  create the Group (Part 1-SHIFT-Part 36).

christopher_owens

Sooo... now I want to put that "Deck Of Cards" Group in another Assembly. Only the Group doesn't show up as a choice to place in another Assembly!! (Bet if it was created in a Parts Studio it would!). But I can place an Assembly in and Assembly...sooo I placed the "Deck Of Cards" Assembly in the final Assembly. Hmmm....

christopher_owens

AH! Since there is no "Copy to Clipboard" for an Assembly, I can Export the "Deck Of Cards" assembly to a x_t file and then switch to another Document and Import that x_t! So now that can be assembled in an assembly in that Document. Now I have a deck of cards sitting next to my sunglasses. Somehow this going to come in handy!

christopher_owens

I keep thinking of a company logo or a "Maker's Mark" (not the bourbon whiskey) that I would want to put on components. Like a "Drag-n-Drop" from one Parts Studio/Document to another. Or "Create Part from..." and select a file. Then use that part to create a Boolean-Merge or an Extrude-Remove.

jakeramsley

We do not have group in part studios.  The idea of group is to move everything as if it were a rigid body in an assembly (essentially a fixed in place relative to one another).

In an assembly, doing a shift + select should select everything between it in the assembly tree.  If possible, can you share the document?

The other thing that you can try, is with the group dialog open, cross-select all of your parts.  If you click+drag from right to left, anything that touches that window will be selected.

christopher_owens

I have used groups in the past for "Bolt-Washer", "Nut-Washer", "O Ring-HYD Straight Connector-O Ring", etc in Pro/E (Caterpillar). Of course, there you could save a file and bring them back in as a group, and then keep them a group or separate to individual parts ( for BOM quantities) with the assembly constraints. Great quick way to build a hydraulic lines assembly for example. Those were always assembled using coordinate systems. I used a group to "back up" or "copy" my larger assemblies! I could drop the group file into a new assembly and remove hoses and connectors that weren't needed in that machine option.

The way Onshape workflow is, you can model up all your parts in one Parts Studio. I think it is the Pattern (Linear or Circular) of parts in a Parts Studio that the Group option may be needed.  I see I can't make a Pattern in an Assembly, say for "Bolts-Washers-Nut" in a bolt circle? I can see where you could Group the components... now would that Group have its own Mate Connector?? So I could place the "Bolt-Washers-Nut" quickly on every hole in the bolt circle?

christopher_owens

I may be getting a bit ahead of Onshape(BETA)! I am use to creating assemblies to generate BOM's and drawings for the assembly line/parts book.

christopher_owens

AHHH! So a Group in Onshape is parts that are not "assembled" to each other, but "floating" relative to each other. But when put in a Group when you move one the other also moves. I "assembled" my 'Deck of Cards' to my 'Card Tray' using "Fastened Mate", after that they would move together. I created a Group out of the two, and the "Fastened Mate" turned red! "Mate is between members of same group". I must unlearn! I did try to see if I could assemble that group into the assembly again. Nope! So if I did Group a 'Bolt-Washers-Nut' I couldn't use that to finish off the bolt circle.

christopher_owens

AH! I see if I suppress the Group, then I can move the parts individually again. Once I unsuppress the Group, the parts move together again.

Auke_Smit_SIL

jakeramsley said:

We do not have group in part studios.  The idea of group is to move everything as if it were a rigid body in an assembly (essentially a fixed in place relative to one another).

In an assembly, doing a shift + select should select everything between it in the assembly tree.  If possible, can you share the document?

The other thing that you can try, is with the group dialog open, cross-select all of your parts.  If you click+drag from right to left, anything that touches that window will be selected.

but is it possible to "group" all parts in the part studio or put them in a folder (in part studio) for the sake of overview?

3dcad

I think it would be nice if you could RMB whole part studio tab and select 'Create assembly' (like you can create drawing) and it would start new assembly, add whole studio in, group all.

If you agree, please vote https://forum.onshape.com/discussion/6490/create-assembly-of-part-studio-using-rmb-menu-in-tab-explorer

@christopher_owens
You can also box select everything and then group (box select is faster in assy than in ps since it only searches for parts).
To copy assembly, select all lines in 'feature tree' - copy - begin new assy - paste (this could also have it's own feature, but let's first wait for assembly configurations)

dave_c

To add a little context and "best practices" to this discussion, Onshape's multipart part studios are optimized to bring the power of parametric modeling to designing multiple parts that have meaningfully interrelated shape relationships.  A general way of thinking about it is - as a general guideline, part studios are for designing shapes, and assemblies are for assembling products.

We at Onshape believe that design multiple parts with one parametric history (aka in a Part Studio) is a major and unique benefit that greatly reduces the work required to design and edit parts with interrelated shapes.  

But it can be easy also use part studios to construct full "assemblies", but this can have serious drawbacks if it is used to design multiple parts that are not very interrelated, or to "insert" and position read-only components (like fasteners).  You can end up with one parametric history with many features doing many unrelated things - and this makes editing each of those unrelated things regenerate slower and less independently (and thus less can be harder to change one thing without changing another).  What is powerful in one situation can be hard to manage in another.

Assemblies are optimized for a) reusing parts defined in part studios, defining the structure (hierarchy and sub-assemblies) and reusing them, and for defining physical behavior like movement, etc.  Because assemblies do not have a parametric history, the bigger they get, the better the relative performance and common operations such as delete instance, add instance, reposition instance, replace instance, create a subassembly in place, reuse parts and subassemblies, etc., are natural and fast.  All of these things are important to defining products, even if they have no or few moving parts.

If you find yourself doing a lot of insert parts features and transform features, or patterns where the results are meant to be instances of the same part, or with parts defined in one studio that are not meaningfully driven by shared sketches or edited by shared features, or with very long feature lists, then you may want to consider using more part studios to define your parts.  

Parts Studios can be a good way to design "top-down" and so can in-context modeling in an assembly context.  Both have strengths.  In-context scales well to nay size assembly and is often the only choice if the assembly is already built.
  
There is no simple one size fits all answer to when it is better to design multiple parts in one part studio vs multiple.  Onshape provides powerful tools, and usually when that is the case, different approaches can be used to solve the same problem. The user is in the best position to decide what is optimal for his specific design situation.   Our customer success team, our support team, and users on this forum are good sources for advice and best practices if needed.