Mirror body method
I don't think so. there is no active plane construction plane unless you are sketching.
you can turn on the origin and use any of it's planes. or a face of a body without adding extra planes
mirror can be used on faces, bodies, features, and components. so make sure you have the appropriate type selected
I also recommend watching some of these videos if you haven't seen them yet. the first one does a good job of explaining how fusion is different..
Let's go through this one by one.
1. You should have fixed these warnings (yellow icons) and errors (red icons) in the timeline when they ocurred. Ignoring these is going to make life much more difficult down the (time)line.
2. Your sketches are almost fully undefined. You should use dimensions. For the slats you may want to consider using a pattern.
3. You are using a skeleton sketch to make the cut-outs for the slats, but instead of using that same sketch to make the slats you create one slat body, then pattern is and because the pattern does not match, you move each body individually. This is very inefficient.
In general Looking at your design, you are using a sort of skeleton design, where you create several bodies from one sketch. Perfectly fine.
However , all of those bodies should be turned into components and perhaps assembled with a rigid group. Review Fusion 360's R.U.L.E #1
Then of you do need to move stuff, move components, not bodies.
I might work on a screencast to see how this can be done more efficiently.
Your sketching technique is questionable. Drawing rectangles with overlapping lines will cause trouble when trying to fully define/constrain a sketch.
I am also wondering how you managed to draw sketch geometry without constraints. e.g no horizontal/vertical constraints.
I've cleaned the sketches from all double, fully overlapping lines and aded all necessary dimensions.
See if what you can learn from going through the timeline. There are many ways to design something like this. I simply used the sketches to their full potential. So if you change the dimensions in the sketches, that's what drives the rest of the design so far. It's not fully debugged. I'll leave that to you 😉
@smallfavor wrote:
I see how you avoided overlapping lines by creating a U shape with constraints. Did you use the pattern tool to distribute them?
Next there's an extrusion for the sides but I see no move record. When you create extrusions from the drawing when how did you place them?
Next it seems you extruded all the slates from the drawing and converted them components - yes? I'd originally done the same but I thought creating a component first and making copies would give me an easier time making changes to the width.
Next it seems you created a component then copied and pasted all the base parts into it, made a group and then - what's 'rigid group;?
Then the mirroring plane - did you place that by offsetting it or was that done with the plane along path or what ....?
I see how you avoided overlapping lines by creating a U shape with constraints. Did you use the pattern tool to distribute them?
Yes,
Next there's an extrusion for the sides but I see no move record. When you create extrusions from the drawing when how did you place them?
When creating the extrusion it does not have to start at the sketch plane. It can start and stop at an object, the two blue highlighted sketch points in the screenshot.
Next it seems you extruded all the slates from the drawing and converted them components - yes? I'd originally done the same but I thought creating a component first and making copies would give me an easier time making changes to the width.
That depends 😉 That's the reason I dimensioned only one slat and then use the pattern tool to repeat that profile.
Now when you change the sketch dimensions, the slat dimensions and associated cuts in the rail (or what ever that's called) change as well.
However, the disadvantage is that when you make a BOM, all the slats are called out as individual components, not as one component with a quantity.
You can still only extrude one slat, convert it into a component and then create a component pattern with the same distance as the pattern in the sketches they always align.
Then the mirroring plane - did you place that by offsetting it or was that done with the plane along path or what ....?
The bottom horizontal line in the Base_Rear sketch has a vertical construction line drawn at the middle point. I created a "plane at angle" at 90 degrees. Whatever the width of that rear profile is, that plane will always be at the middle of it, s that's what I am mirroring about.
In general in a parametric design I try to avoid moving bodies.
