Fusion
Are there any issues highlighted in yellow or red in the Timelne?
This is a pretty rough model - I would be surprised if it DID shell.
Stop and ask questions at the first sign of trouble. This will take some time to diagnose.
Edit:
First thing I would have done is place the import with symmetry about the Origin.
Sketch1 is very very rough. Already building a house of cards on a foundation of quicksand.
Use lines and arcs if possible (fully dimensioned and constrained) rather than splines.
Certainly, don't use multiple splines where a single two-point spline will suffice.
What is this number?
Most designs exhibit significant symmetry.
I do not see symmetry in your Sketch1?
Hi,
I find the easiest way to create a shell is to use the Surface commands.
The easiest way to do this would be to create the shell with the Offset command
and use the surface of the object as your body to get the initial 1mm Offset,
And then use the Thicken tool to create the 1mm thick new surface.
I have created a simple cube as my original body and created a shape that
is 1mm from the cube and 1mm thick.
Cheers
Andrew
Hi! Since this is a mesh model to begin with, you may use Mesh Design environment to edit the mesh. You may use the Shell command in Mesh Design to create the hollowed mesh.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
@colemanHEXZG wrote:
I've uploaded the model as it stands now
My first thought is why did you scale the import?
This moved it away from the Origin.
I suspect that you had the incorrect units set on import.
Let's start with your sketch labeled Sketch2.
You should probably forget about Mesh Section for now - it is not useful with this scan data.
Blue lines should keep you awake at night. STOP on any sketch that has blue lines. Do not continue. Ask questions.
I see a lot of Mirror (or Symmetry Constraints). There is almost always a more computationally efficient technique.
I see an inside and outside offset sketch geometry - not needed. Keep sketches simple. Probably don't even want the Filets in the sketch, but for now we will leave them in.
This dimension is impossible to measure in the real world and therefore does not make logical sense.
When I add the missing dimensions - none of them make logical sense. Not one!
Note that when the sketch is fully defined with dimensions and logical geometry constraints that it turns from blue to black.
It might seem like a lot of extra work, but actually, when done properly - Fusion does all but one of the geometry constraints for you.
The only thing you need to do is enter logical dimensions.
Note: It should not escape your notice that you have not been offered this logical information by the experts here in ANY of the previous responses to your queries.
I quite frankly can't understand that omittance.
Maybe it was a lack of information in the original problem descriptions.
My initial impression is that this is a scan of a commercial product.
I know that you stated that you only have access to the scan, not the physical model from which it was made, but can you identify this product?
Some photos of the actual product somewhere on the internet?
Photos along with the provided scan would go a long way towards making this reverse-engineer easier.
In Sketch2 you have an arc that is very very close to being a straight line.
Now if you intend for an arc, that is fine, but it is so close to being a line that I have to wonder about the true Design Intent?
Highlighted blue at the bottom. 0.04 mm from being straight line.
