Cannot use fillet after creating solid via sweep tool.

[j.lanoszka]

Hello,

Is there any way to use a fillet or some other tool to create a round edge on solid that was made by sweep tool ?

I think sweep tool is the only tool that provides me exactly what I want so I am not considering other tools for creating my solid part.

Every tip is appreciated. Thanks.

[JDMather]

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@j.lanoszka wrote:

I think sweep tool is the only tool that provides me exactly what I want so I am not considering other tools for creating my solid part.

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I do not see a Sweep feature in the part that you attached.

Did you attach the correct file?

If this is the correct file and you meant to write Loft rather than Sweep - 

what size Fillet to you want?

On bottom edge only?

[JDMather]

Maybe something like this?

[j.lanoszka]

Yes exactly. I meant loft of course not sweep. My mistake, sorry.

Yes, I want it on bottom surface, just as you did it.

Could you please explain how to do it, cause I receive error like this below:

[JDMather]

Did you look at my file?

Your sketch was very rough and not fully defined.

I started over from scratch.

[johnsonshiue]

Hi! I think this part can be done without using Loft. I guess this is a modeling sequencing issue. The rounds (fillets) should be added after the shape has been defined. Adding detail geometry too early can lead to unnecessary complexity.

Please take a look at attached part. I remove the rounds. Then simply extrude it with a taper angle. After that, you can add the fillets to those edges. The geometry should be much easier, precise, and clean to work with.

Many thanks!

[j.lanoszka]

Thank you Johnson for your advice.

I've got one more question about this part. Next step I need to do is cutting a specific shape on the curved face of the part. See picture in attachment. The cut needs to look like sketch_10 and 2mm thick into the part.

I think I've tried everything but achieved no success at all. I'm only able to cut this part just like I upload it here with the use of sweep tool, but I do not have any idea how to get the profile like on sketch_10.

[SharkDesign]

Why are you using sweep to cut this?

Start a sketch on the sloped side, project the sketch onto that and then cut it.

I'm assuming you want that entire inside area cutting into it?

[j.lanoszka]

Can you do it on attached file and upload it ? Then I tell you if it is what I want.

[JDMather · Accepted solution]

Create a 2mm offset surface body.

Extrude-Cut to the surface body and then hide the surface body.

See Attached.

[johnsonshiue · Accepted solution]

Hi! This can be done in multiple ways. You can also project the 2D wire to the face (in 3D Sketch). Then use Split command -> select the 3D curve to split the face. Lastly, use Thicken -> Cut to create the dent.

Many thanks!

[j.lanoszka]

This part drives me crazy.. Now I am not able to create a shell after using sweep tool. Anyone wants to support again ?

Many thanks.

[johnsonshiue]

Hi! Shelling should be done before detail features (fillets and chamfers) are added. For your part, right after Extrusion 8 is a good place to create the shell. I am able to shell up to 4 mm.

Many thanks!