Hello,
I'm trying to stop a body from entering the space of another body when moving it across the workplane, is there a way to achieve this? I.e. I'd like to stop two bodies from overlapping each other.
Thanks in advance,
Regards Jan Gunnelin
Solved! Go to Solution.
Solved by TrippyLighting. Go to Solution.
Solved by jan.gunnelin. Go to Solution.
Solved by TrippyLighting. Go to Solution.
Solved by TrippyLighting. Go to Solution.
You can prevent that by not moving the body you are moving.
If you have components, and not bodies there are many ways to do what you ask.
Try a screencast to show us the problem.
Hello,
Thanks for the quick feedback! You are correct, it is components that I try/should try to move without interfering with each other. Please see the attached screenshot with a red and a white component. They should end up side-by-side, not overlapping each other.
Regards Jan
With Joints there is the offsets section of the Dialogue.
When you select the Components, you are asked for reference points, then you set the Offset to separate them.
Might help....
I tried your proposal and it works fine! But I need to do this in two dimensions simultaneously, and then it can't help me, I loose the joint created in the first dimension when I activate a joint in the second dimension.
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.
More screenshots, will stop our guessing being off the mark,
Joint Offset allows three at the same time, I can’t see the problem so far.
@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.
Thanks so far! I'll be back with more screenshots later on! I will try out joints a bit more also.
Hello again,
I have attached two screenshots. I tried to attach one exported file (I could not find the option .f3d as requested but exported an .f3z file via the Fusion webinterface instead). I failed for unkown reasons. Anyhow, the leftmost figure shows a manually correctly aligned combination of a large and a small corner. The middle figure shows manually misaligned corners and the rightmost figure a failed attempt to align the corners with two joints. The second joint breaks the first joint as I understand the situation.
Regards Jan
If you were starting with the red component, and decided to build the bone coloured one in place,
one would need a sketch for the corner of the bone component. Project it (the Apex sketch position,) into the red component.
When not built in place sketch the destination position in the red component. (One line would be enough.
Use the apex on both components,
Might help.....
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.
This example was just an illustration of my need to reuse a large building block including a white angle in a number of other large building blocks including a red angle. When the building block including the white angle is derived for use in another building block, it "lands" somewhere on the worksheet and then needs to be moved to a target location with ease and without colliding/interfering with the target component.
Here is a link to the CombinedCorners design example:
Hi davebYYPCU,
Thanks, I'll experiment with sketches and apexes a bit!
Regards Jan
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.
Hello Peter,
Thanks for all your efforts in helping me out, including filing bug reports! I really appreciate it as I'm a newcomer to Fusion 360, I have just recently moved to it from TINKERCAD. To set and edit a Joint Origin can probably be a viable way forward for me, I just tried it for the first time and it seems to work! Thanks for the hint! 🙂 Here's the latest version of the CombinedCorners experiment:
I can't see or find out the difference between Derive and Insert in my Fusion 360 Model view, please see the attached "AvailablInsertCommands" screenshot.
Regards Jan
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.
Can't find what you're looking for? Ask the community or share your knowledge.