Creating a slope along a circle
@Davidf01, there are multi ways to create a sketch.
1. Start most all sketch commands (create sketch commad or project, line, etc.), then the work planes show up, you can select work planes and also a face on a body. Please let me know and help to capture an image if it doesn't work. Thanks!
2. Right click mouse to select a face first, then click "Create Sketch"
@Davidf01, yes, Fusion supports inserting one design into a another design, which is XRef/distributed design.
As below image, right click the design on data panel (or drag it to graphics canvas) to insert it to current opened design (need to save first). The inserted design is a reference, need to open it to edit, so in your case, you could right click inserted design in browser and use "Break Link" to fully import the design contents into new design file.
Could you also share your file which has the issue, we could try to check what the problem is ? Could you also double check whether the "Body Faces" filters are checked? Selection Filters are used control what kinds of objects are selectable in order to select specified type objects easily.
@Davidf01, the reason is that the top face isn't exactly a plannar face, sketch requires plannar face.
I tried to make the sketch line as below to horizontal/vertical, and then edit the revolve feature (by remove axis and reselect it again). Then it works. Please take a try and share any further comments, thanks for sharing the file!
Make the sketch line as horizontal/vertical, to make sure resolved top face are plannar.
Edit Revolve feature by remove axis and select again
Hi Davidf01,
glad you're making some progress on your design and that you're getting some great tips from Jesse (jjurban55) as well as some other Autodeskers.
So I took a look at your design and a couple of observations:
my first one was that you are likely going to do some sort of polymer production process: rtv mold, injection mold, 3D print-maybe!?, but probably not thermo formed (too thick a part).
Considering the first two options mentioned above, I see a couple areas where your model will need fine tuning to get a proper mold made, and that is drafting your model to get a uniform finish on your part and to get the finished part out of your mold without marring your finished surfaces.
So I wanted to show you another way you can get the result I think you're after.
in the image below I'm showing a sketch that matches your design intent sans corner radii, as I added them as solid modeling features rather than sketch elements.
The one thing I like to share with beginner users is keep it simple.
Try and distill your sketches to the most simple, base geometric form whenever possible. In the case of your mug lid, I had forgone the relatively complex sketch in your model and just used a simple circle to create the first two features that are the base of the lid design.
Build your design as primitive geometry and use the power of the modeling features to add detail; rounds, draft, shell for part thickness, etc. Although your design is not too complex, keeping this sort of detail out of the sketch when you're working with more complex designs will serve you well if you have to troubleshoot a failed feature in more complex models. In time you'll learn how much detail you can add in a sketch to capture critical design intent and where you can rely on the 3D modeling features to get the intent you want, there is no magic formula here, but keeping it simple is a good place to start.
Feel free to play with the example I built and step back and forth through the timeline to see exactly the steps I took.
hope this helps.
p.s. the "hollow" look in your cross sections is from the ambient occlusion setting, turn this off and all should be good. Also to create a sketch on an existing surface the surface has to be planar, if the surface has any "out of flatness" you can't sketch on it.
Jamie Gilchrist
Senior Principal Experience Designer
Man I'm learning a lot too, that's an awesome idea! Here I extruded a simple Tspline cylinder then used Modify to move the node points up or down. Next I created a sketch on an arbitrary plane and used Include 3D geometry and selected each top edge segment.
which is available then in Model or Patch environment to create a sweep:
The Patch sweep can be a little picky about fully closed loops which is easy enough to work around, but found in Sculpt environment didn't have a problem creating a closed loop sweep. Note in both of these, going around the loop in one direction can give a strange result, whereas then trying the other direction worked fine.
I also wanted to try extruding two cylinder Tsplines, and then selecting two adjacent node points at a time, would move them up or down together.
The resulting two curves can then be used to insure the loft in this case stays level along the path (note choosing rails in the loft tool is a little tricky, be sure to uncheck Chain, and add a new input button for each rail).
Again really great idea you came up with David!
Jesse