A moved part goes back to origin during editing - how to stop this?
@melvinbrian3d I know what you are going to suggest, but thats really not a recommended practice.
@Anonymous This is normal in designs that use a bottom up design process. When you edit a feature or sketch you travel back in time to where that sketch or feature was first created. You should however use the joint in the assembly menu and not the capture position feature to get your parts assembled correctly.
The occasional use of a position capture feature is OK, but frequent use can create performance problems.
In general you'l have a lot less problems if you follow a top-down design process and create your components in place.
@TrippyLighting was not suggesting using external linked files.
You have 2 options.
1
Create a component then just create the sketches, extrusions etc. in place and never move the component and don't worry about the origin remaining at the document origin. Probably should ground the component or add a rigid joint to stop it moving.
2
Create a component then use a joint to position it. Turn on the component origin pick the joint tool select the components origin then the destination point. You might need to create a joint origin for the destination. As trippy said don't use capture position as it stores the position of all components at that point. As the joint is the first feature in the component you will never have the component move while editing it's other features.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@Anonymous wrote:I created something simple just to test the recommendations but I deleted it.
I'll create a new one and will share.
Never shared before - how should I do it? - Share public link (under File-Share command) or Share to Fusion 360 Gallery?
just Export and Save The File .F3D, and then upload the file here
MelvinBrian3D
i hope i've understood correctly,
this is what you want?
here is the Version 4 with the sketch and revolved moved further in time and constrained with the new point of the square sketch.
MelvinBrian3D
@Anonymous wrote:correct me if I am wrong, but in your V4 model you did not re-constrain the Collar to a new point in the Base but you just moved the sketch of the Collar further away form origin. Am I correct?
The constraint is still the same to the same old point?
It would be acceptable in many cases, but sometimes the Base can get modified so much that this would not work. For this reason it is our company policy not to move sketches from origin if part does not change.
Hi, I re-define the collar sketch plane to the new point you created as you can see in this picture
MelvinBrian3D
@mavigogun wrote:
@TrippyLighting wrote:
The occasional use of a position capture feature is OK, but frequent use can create performance problems.
Please, elaborate- what concerns and considerations/implications should we be mindful of regarding Capture Position?
The capture position feature captures the orientation and location of every component in the assembly that has moved since the last position capture feature was used. That can accumulate to a good number of calculations.
If you have a parametric design with user parameters and change a user parameter, Fusion 360 has to re-calculate the timeline and all position capture features have to be re-calculated. That can result in performance problems and make a design slow.
A while ago I removed a lot of those position capture features from an older design that were not really needed and it sped up the re-calculation significantly. But, again, occasional use is fine.
@Anonymous wrote:
For this reason it is our company policy not to move sketches from origin if part does not change.
I am assuming that policy is not based on the feature set present in Fusion 360 ?
If you design parts in place then all component origins will coincide with the top level origin.
A sketch for component B ( the collar for example) that is created on a face of component A (the base) will not be coincident with the origin in all axes.
Are you familiar with the BORN modeling technique ?
@Anonymous wrote:
I never design in place in other CADs (primarly the I-Deas).
That is the reason you are struggling with Fusion 360. It's not that you necessarily have to design components in place, but top down design is really Fusion 360's strong suit.
Every CAD software requires some adaption of workflows and Fusion 360 is no exception to that.
No car or airplane is designed using a single CAD system. The cockpit of a modern Airliner can easily have several 10k components. A vehicle as a couple of then thousand of components.
While I've not worked int the aero space industry (yet), I've worked in a vehicle plant (BMW) directly with the design engineers . In the automotive industry CATIA is the predominant CAD tool.
You hopefully are not seriously comparing an entry level CAD tool to CATIA.
No, of course you would not attempt to design something of that complexity in Fusion 360. Neither would you be able to do this with Top Down design methodology alone. None of the things I design are purely Top Down design. That applies to the automation concepts I develop or the LED art I create or the freelance industrial and product design work I do.
The rule of thumb is that Fusion 360's limit is about 1000 components. Even designing a small machine can quickly reach that amount of components. Reorganizing the assembly structure in the browser is not very efficient and can only be done with the timeline rolled all the way to the end.
The fact, is however, to find the limits of what you can do with Fusion 360 you'll have to actually use it in a few projects and adapt your workflow to the way Fusion 360 works. It takes a little while.
Many ot the things you feel are a problem now won't be down the road.