How can I stop a body from entering the space of another body?
@jan.gunnelin wrote:
Hi Peter,
I can't share my design at the moment but you can think of it as a smaller corner that should fit inside a larger corner (in two dimesions initially). The smaller corner shall not interfere with the larger corner, i.e. just touch it seen from the inside of the larger corner.
Then we shall reconvene when you have time to post your model.
Before giving any recommendations on a better workflow I would need to understand what the overall goal of the design is.
For example I don't quite understand the need to use derived components in a design that looks fairly simple at this point.
There;s no need to export anything. For distributed design you can simply share the public link to the design, which can be retrieved from the design on the data panel.
I looked at your design and you may know this already, but I am going to mention it anyway.
The sketches In your individual components are not fully constrained and dimensioned.
They are also not constrained to the sketch origin and that is never a good idea.
This sketch is fully defined and the sketch icon in the browser is equipped with a little red pin if it is fully defined.:
Then it really only makes sense to use "derive" insta of "insert" for external component if you actually intending to modify this components in the assembly. If not, then "insert" dos the same thing, but has two advantages. It is less data heavy and uses less computational resources. You can inert a component into any subassembly level you want to. But derive goes currently always into the top level ( that is a real bummer IMHO).
The next thing I'd recommend is ....
Hang, on. I just ran into a bug in this awesome software that was reported a few years ago ( a number of times by yours sincerely) . I need to see if I can find a nice workaround.
I filed two bugs in conjunction with the workflow I was going to show.
1. These component done;t really have geometry at those points where one would want to join then, so this would be a good opportunity to add an explicit joint origin just for that purpose. It does work, but ...
when you edit the joint origin it looses it;'s connection to the parameter.
Let's not edit joint origins then and move on to the next problem.
2. When you then open the design that these components are derived into, you need to update the components.
Then you'll find that you won't find the joint origins in these derived components. That's another bug.
So if you're happy with not editing joint origins and can use "insert" instead of "derive" then we can continue down this road.
Otherwise I'll have to come up with a more convoluted workaround.
Looks like I never posted the result of my experiment. I only call this an experiment because the bugs in Fusion 360 made it more difficult then it needed to be.
What I did in the designs for the individual components is to add an explicit joint origin. this geometry is a very good candidate for the use of these explicit joint origins, because the geometry does not one any convenient snapping points for the implicit joint origins that are cerated during the creation of a joint.
I just extended the sketch in the design so I had point to reference for the joint origin.
The creation dialogue allows to offset the joint origin and I used the parameter for the diameter. "d3" (divided by 2) to offset the joint origin to the desired location.
Then I turned off the sketch. The visibly of explicit joint origins can be turned off in linked designs, as opposed to sketches.
In the assembly I created a subassembly that contains both of the parts, joined to the origin of that assembly "Asm".
Then I joint "Asm" to the main origin and patterned it.
Of course if this would be an irregular pattern then you could create a sketch and join the joint origins to points in the sketch.
Here's a link to the design.
