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Assembly - Insert Plane from Part studio
james_close
Member Posts: 19 ✭✭
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.
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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
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.
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
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.
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
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
IR for AS/NZS 1100
I did not try that originally ( mentally stuck in Solidworks mode).
I just did and found the following, more testing required on my part.
Thanks,
Jim
I'm going to piggy back here that having planes in an assembly would be VERY useful and quite powerful for automation and modularity. I've got my fair share of experience in CAD software (all the way from autocad to Catia) and they're absolutely essential. I'm baffled to read all of the above if I'm being honest. I feel like some people at Onshape don't have an extensive enough pedigree to judge on the pertinence of some features.
I do hope the PM will pick up on that someday as I've literally changed multiple time from onshape to other softwares (SolidWorks, Fusion360 to name a few), simply because the assembly did not offer very strong features. Hell, there's not even an "in-between" feature to center a part between two other ones.
You do realize that Onshape was founded by many of the same people who founded Solidworks? There's a great depth and breadth of experience there.
There are occasionally things where some early decisions are still a bit annoying to many. I will definitely agree that assemblies need some sort of easier to grab references for mates and cross sections. It's one of the more user-hostile things that they cling to.
That said, there are so many things that they got right with how history/versions/branching/merging/references etc work, that I constantly forgive some of the oddities. In fact I do not want to go back to other CAD systems.
There is a "in-between" mate, BTW. It's called "Width mate". The only frustrating aspect is it doesn't handle things like a U-shaped channel with draft on it very well. For that, you need a second mate. In general, if you find yourself using more than one mate between two parts, you're likely doing something more complicated than necessary.
https://www.onshape.com/en/resource-center/tech-tips/center-parts-using-width-mate
Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn
When I say some people, I'm not pointing fingers at the CEOs, as their role isn't really "technical focused". I'm saying that it's odd that some very important features seem to be missing entirely while they exist in all of the other softwares. Sure, the kind of "git" tree is pretty interesting, but so is the PDM from solidworks. Vaults and versioning aren't ground breaking in CAD. There are no perfect softwares out there. If Onshape had it all, I doubt we would see that many competition around.
Good catch for the width, even though it was added quite recently. Anyways, I'm not here to start any kind of friction. I'm simply baffled the features aren't there YET.
Remember that there are implicit make connecters on many locations on every part. There are no explicit mate connecters in this example and no work planes in the assembly. One thing that helps to start this off with the main body to work around at the origin so that it can be dropped on the origin then fixed. Don't drop and drag first part, just pick and hit the check mark.
@james_close
I hear ya. Decades of using top down design in Creo… trying to reprogram my brain for OS. I was totally baffled that I couldn't put a symmetry plane in my assembly. Yesterday I had the revelation that the X-Y of a "Mate" is a plane that can be used for that purpose. I guess the the Mate nomenclature through me off.
Don't have all the answers, just chiming in that I feel your pain.
@vincentpelletier1 Onshape does have default planes and the ability to make planes and axis in assemblies.
Remember, a mate connector is a [Point] [XY Plane] [XZ Plane] [YZ Plane] [X Axis] [Y Axis] [Z Axis] all rolled into one feature.
If you want more construction planes/axis/points you can just add a mate connector here:
When you try to mate to the origin, you have the option to use all of these, just hold shift while mousing over and you can grab the other options easier.
When you try to mate to a mate connector and access these secondary functions, you may have to edit the mate.
Here is an example gif showing how to use the origin as a Z axis for the pattern, and all the planes to mate the tubes. I don't ever recommend doing this… Onshape has better mating options than planar... As I show in the end the video, when I delete all the mates and just fix / group the parts, taking literally 2 seconds, rather than a minute doing the SolidWorks way.
And stop trying to run Onshape like "other CAD", learn how to properly use Onshape and you will forget why you ever thought you needed a plane in an assembly ever again.
Here's a nice sample from Too Tall Toby. Good explanation.