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I have finally made this perfectly and fully constrained "tile" with joints. The idea is to 3D-print a bunch of such tiles, such that they can strongly and permanently joined together. You may discern that the receptacles have some clearance compared to the plugs.
Now, having drafted two sides with all relevant constraints, I would like to mirror the entire geometry to the other two sides. I cannot figure out a way to do that. At the very least, I would like to mirror the sketches. In an ideal world, I would also mirror the bodies, but note that they would have to be turned around - because otherwise a plug would encounter another plug rather than a receptacle when joining the tiles.
Any advice would be enormously appreciated!
Mirror the extrude features in the timeline. In the mirror dialogue you can change the pattern type to feature and then select the features in the timeline
I have a follow-up question. I have now generated some walls (see pic), and would like to apply the same pattern of plugs.
However, the vertical wall is now a separate component called "vertical corner", which is probably a bad design decision. I have done that because the three bottom tiles are parametrically linked, and therefore anything I draw on one tile will propagate onto the others.
What would you advise me to do?
- I could unlink the tiles from each other ("paste new", I suppose) but that is logically incorrect since they should all simultaneously update their dimensions if I decide e.g. to make them thinner or thicker.
- If I however stick with the vertical walls as a separate component, I cannot simply do a circular feature pattern from the "tile" component onto the "vertical corner" component. Right?
- Or (hopefully) there is a more elegant strategy that I haven't identified?
For any advice I would be most grateful. I have to say that I find this community to be amazingly supportive and friendly. Be assured that I'd be happy to reciprocate (I am however a medical doctor by profession).
@AagAag wrote:
As you probably surmise, this is primarily an exercise by which I am trying to learn how to do strict parametric drafting.
Well, yes we've gathered that much. The question is who is actually exercising. I don't see you producing much other than text while @chrisplyler is spoon feeding you with the patience of an ox.
If you don't really start experimenting seriously yourself you can watch other people's screencast until the cows come home but you still won't be able to complete these simple projects.
Now I have to apologize for being irritated!
Allow me to back up my apology by doing some good ...
I downloaded one of your designs. And I am looking at the first sketch, which is almost fully defined.
It contains one spurious line that is not constrained to anything. I am sure that was my accident, but I am going to take the opportunity to warn of overlapping lines. Avoid these as good as possible.
Imagine you'd have to sketch everything in ink on soft paper. You never want to go over the same line twice.
That is also a good practice when sketching in CAD.
The second think I am noting is that you sketched the profile offset by a fixed distance of 35mm. Form a "standard" reusable part I would keep the origin of the design located at the center or corner of a face, vertex or body. This will often help not to have to create auxiliary construction planes for mirroring, or axis for patterning.
Also, if parts are symmetric it is usually a good idea to have the symmetries align with origin axis or planes.
You mention 6 parameters in another post. I believe you need another 2 parameters for the 3D rating clearance.
I am assuming these will likely be printing flat on the printer bed with a FDM printer. The tolerance in the Z axis is usually smaller than in the XY plane, hence 2 parameters.
In your sketch that would mean that you cannot use a uniform offset to allow for that clearance.
Another question you asked was in relation to sketches not being located in the component they should actually be in.
This can be done, but in your case you are too far along in the design and relationship exist between some entities in the component and outside of the component that prevent this from working. Unfortunately there are currently no tools available to untangle this.
It might not be a problem. You could simply continue in this design and use it only to great a small library of the tile variants you want to create. Then you can use a feature that was only recently introduced to Fusion 360. The Derive command allows to derive components from one design into another.
So you can derive one or more tile variants out of that small library into a new design and use it to build something with these tiles. the advantage this hs is that if you need to change the printer clearance, you change the user parameter for that in the library file and the designs with all the derived tiles will update to match.
@chrisplyler wrote:
The downside is that if you want to save each Component type out as it's own file, they aren't going to have the sketches included with them.
True, but with the new derive component functionality you can keep a library file with just the tile variants and then derive these into your those design where you use the tiles to build something.
If there are not too many tile variants in that library this should work nicely..
Correct!
The reason I mentioned "small" library is that if you update a library file that contains a number of your tiles, even if you only modify a single design, all assemblies that any component/tile was derived into from that library file will also have to be updated.
So if you library grows beyond an hand full of parts you'll have assemblies show the need to be updated when there is really no change. Fusion 360 keeps versions only of complete files, not the component in that file.
Thus I would not use the derive functionality for a growing and constantly changing library of re-usable parts.
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