Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.
First time visiting? Here are some places to start:- Looking for a certain topic? Check out the categories filter or use Search (upper right).
- Need support? Ask a question to our Community Support category.
- Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
- Be respectful, on topic and if you see a problem, Flag it.
If you would like to contact our Community Manager personally, feel free to send a private message or an email.
Options
Why did "Fixed" parts in an assembly move?
jon_woellhaf
Member Posts: 92 ✭✭✭
I created a gear train and "Fixed" all the shafts. I then went to the parts studio and moved several parts and deleted others that are not in the assembly.
When I returned to the assembly, all the parts were still there, but many had moved.
Why would making changes in the parts studio change the relationship of the parts in the assembly?
When I returned to the assembly, all the parts were still there, but many had moved.
Why would making changes in the parts studio change the relationship of the parts in the assembly?
0
Best Answers
-
Options
jakeramsley
Member, Moderator, Onshape Employees, Developers Posts: 657 
The assembly is just referencing the geometry and positions of the parts in the part studio and applying transformations on them. When you are fixing things in assemblies, you are saying that you want no additional transformations to happen to those instances in the assembly. By moving the part in the part studio, you are changing what the default position in the assembly is which will make it look like the part moved in the assembly. It is because of this that I suggest constraining parts that are inert with mates to the origin in the assembly so that their positions are solved in a way that makes sense in the assembly.Jake RamsleyDirector of Quality Engineering & Release Manager onshape.com5 -
Optionsjakeramsley
Member, Moderator, Onshape Employees, Developers Posts: 657
Here's a quick example I just made: https://cad.onshape.com/documents/05095da422132c61d8951148/w/26c6cffeb0d4afa605cc3f9a/e/61416b7715fa49c293968c86
No, you are using Part Studios exactly how I would expect. I'm just not being very clear in what I am trying to say.
To continue on with the ball bearing example, imagine you are making one (or have imported one) that has 8 balls in it, so that will be 10 total parts (inner ring, 8 balls, outer ring). These were all designed in the Part Studio relative to one another so that if you were to change the size of inner ring, the size of the inner ring will also increase so that the distance between inner/outer is held the same. The size of the balls won't change, but their position in the Part Studio will, they will be moving out radially from the center of the rings. If this change in position didn't get represented in the assembly, the balls would now be overlapping the inner ring because all that happened in the Part Studio was their position changed.
For example, I have a ball bearing where the size of the gap between inner/outer ring is constant. I added all the parts to an assembly and fixed all of the parts.
If I then update the inner ring to be 50mm instead of 25.4, then everything expands outwards but the size of the balls stay the same. Their position, however has moved. If the assembly didn't respect this, then the assembly would have the balls in the previous position which wouldn't be what I wanted.
Jake RamsleyDirector of Quality Engineering & Release Manager onshape.com6 -
Options
OpenR2
OS Professional Posts: 188 ✭✭✭
Actually Jon has point...although the initial reaction is to say this is standard instance and reference behavior ... its a still a little bit of a struggle to understand what data model Onshape is using in which context.
Since there is what is traditionally assembly modeling happening in the part studio it is natural to think that the part instance and reference modeling in happening in the part studio tab, and that the product occurrence modeling is happening in the assembly tab.
In the part studio the feature tree behaves like a traditional single part spec tree, but the solids with mirroring and such behave 95% like a traditional assembly tree. The assembly tab behaves 95% like a traditional kinematics tree/configuration tree.
What I think most folks are used to is...
Feature tree .... usually in a part
Multi-solid bodies ... usually in separate parts
Part instances ... usually used to store immediate parent/child relative relations
Product occurrences ... usually used to store configuration information and effectivity
My bet is that long term Onshape will migrate back to these 4 standard objects because this is what works when doing product design for automobiles and airplanes.
6
Answers
Another area where it is useful is when importing foreign data that will all be moved relative to one another. For example, if you found a nice x_T file of a ball bearing that you wanted to include in your design. You could insert it into an assembly, group all of those parts together and treat it as a static element. If you then modified the size of the bearing, then it would update the positions of the entire piece in the assembly rather than forcing you to go through and mate everything together.
I am apparently using the Parts Studio differently than you intended.
For example, were I to create a ball bearing from scratch, I would create the individual parts -- ball, inner race, outer race, carrier, rivet -- in a Parts Studio then insert them into an Assembly named Ball Bearing, and mate them appropriately.
I would then expect the ball bearing assembly to remain as I designed it irrespective of any change in the position of the parts in the Parts Studio.
What is the correct way to create a ball bearing?
PS: This forum is WONDERFUL!
No, you are using Part Studios exactly how I would expect. I'm just not being very clear in what I am trying to say.
To continue on with the ball bearing example, imagine you are making one (or have imported one) that has 8 balls in it, so that will be 10 total parts (inner ring, 8 balls, outer ring). These were all designed in the Part Studio relative to one another so that if you were to change the size of inner ring, the size of the inner ring will also increase so that the distance between inner/outer is held the same. The size of the balls won't change, but their position in the Part Studio will, they will be moving out radially from the center of the rings. If this change in position didn't get represented in the assembly, the balls would now be overlapping the inner ring because all that happened in the Part Studio was their position changed.
For example, I have a ball bearing where the size of the gap between inner/outer ring is constant. I added all the parts to an assembly and fixed all of the parts.
If I then update the inner ring to be 50mm instead of 25.4, then everything expands outwards but the size of the balls stay the same. Their position, however has moved. If the assembly didn't respect this, then the assembly would have the balls in the previous position which wouldn't be what I wanted.
Since there is what is traditionally assembly modeling happening in the part studio it is natural to think that the part instance and reference modeling in happening in the part studio tab, and that the product occurrence modeling is happening in the assembly tab.
In the part studio the feature tree behaves like a traditional single part spec tree, but the solids with mirroring and such behave 95% like a traditional assembly tree. The assembly tab behaves 95% like a traditional kinematics tree/configuration tree.
What I think most folks are used to is...
Feature tree .... usually in a part
Multi-solid bodies ... usually in separate parts
Part instances ... usually used to store immediate parent/child relative relations
Product occurrences ... usually used to store configuration information and effectivity
My bet is that long term Onshape will migrate back to these 4 standard objects because this is what works when doing product design for automobiles and airplanes.