Can not Project face and extrude of a components

[17521010]

I need some help with a modeling issue I’m facing in Fusion 360. I’m working on a boat model, and I’ve run into problems with several features — specifically with Project, Extrude, and Combine not working on certain parts.

For example, the boat floor was originally made from a group of surfaces that I stitched together into a solid body. However, when I try to extrude a sketch to cut into it, it just doesn’t work. The same thing happens with the front cabin. I tried to project its face, but Fusion won’t let me select the face for projection. I also attempted to use Combine to join the cabin with another body, but the command doesn’t seem to work either.

I'm not sure if this is due to the geometry not being completely solid, or if there’s something wrong with how the faces were stitched. Has anyone encountered this kind of issue before? Any ideas on how to fix or troubleshoot it?

[TheCADWhisperer]

@17521010 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[17521010]

Sure! Thank you so much for offering to take a look  I really appreciate your time and help. I’ve just exported and attached f3d file here.

[TheCADWhisperer]

@17521010 

I haven't dug deep, but first thing I notices is an illogical angle in your Move.

I would expect zero degrees.

I would not expect to see this tiny offset...

I wouldn't expect to see this...
(I am zoomed wayyyy in this image below.)

I would not expect to see Shell here and in section view it does not look correct.

I got lost after that.

[17521010]

Thank you for pointing that out, i honestly didn’t notice the angle issue until you mentioned it. I’m sorry about that. I’ve reviewed my timeline history bar to try to fix it, but every time I attempt to make adjustments or roll back to that feature, I keep getting red error messages. Do you have any tips on how I could properly fix this?

[TheCADWhisperer]

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@17521010 wrote:

Do you have any tips on how I could properly fix this?

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@17521010 

I added other observations to my previous post.

I recommend that you start over from scratch and concentrate only on the Hull at first.

It appears that you wanted that to be zero degrees.

Therefore, I would rotate/move before doing the Replace Face and use the Origin plane for the Replace Face rather than a 3-point plane.

Extreme care must be exercised to get a clean Shell, and it must be done at the right time in history.

Edit:  I went back to the beginning and attempted Shell before the other operations. It is so slow that I suspect the imported geometry is rubbish.

I recommend not using the imported geometry and instead create all geometry natively from the start.

[TheCADWhisperer]

@17521010 

[17521010]

[17521010]

Thank you so much for the explanation. I’m still a bit confused about how I can avoid making the same mistakes again in the future. It feels like I keep repeating the same pattern without realizing it just like with this last model.

[johnsonshiue]

Hi! I took a quick look at the model. I think it is a combination of preexisting bad geometry and loose tolerance in stitching, which leads to further modeling failure. Here is a proof. I export the two target bodies to SAT (see attached file). Then import it back to Fusion. Turn off Capture Design History and the Validate command becomes available. It confirms there are errors in the Hull body. Then I simply unstitch the entire body and restitch the surfaces using very tight tolerance 0.00001mm (Fusion 3D geometry tolerance). Repeat the process for the other body. After that, they can be combined without a problem.

The result confirms that the bodies have issues. These issues preventing further modeling from working correctly. I agree with JD. I think I would study the model carefully and capturing the design intents. Recreate the whole model from scratch (by reusing certain geometry). The model as is at the moment isn't robust. More modeling issues will be encountered down the road. Certainly, it may take a bit more time initially but the model will be more editable and extendable after that.

Many thanks!