Cant Extrude Sketch from DXF

[Anonymous]

Hi there,

I am trying to extrude a sketch from an imported DXF file. It should be very simple but for some reason I cannot extrude the sketch. Fusion 360 does not allow me to select the shape when using the extrude tool. Any ideas what I am missing?

I cant attach the DXF to the forum, it says: 

Correct the highlighted errors and try again.

The attachment's dxf 2 extrude.dxf content type (application/x-dxf) does not match its file extension and has been removed.

I have re-exported the DXF out of Fusion 360 from the sketch so the DXF file itself should be okay. I can't understand what the problem is.

Thanks in advanced for any insight you can offer..

[MoshiurRashid]

HI

Thanks for posting. From my side, I think there may be one of the two problems.

1. In the sketch palette the "Show profile" is not checked. (Go to edit sketch to find the sketch palette)

2. The sketch is open in somewhere.

For more, please share the f3d file here. (files> Export> f3d)

[g-andresen]

Hi,

Please share the file.

File > export > save as f3d locally  > attach it to the next post.

günther

[Anonymous]

Thanks for your replies, see attached.

[g-andresen · Accepted solution]

Hi,

close the open corners (white dots)

Unfortunately the light blue colouring of the profile is not visible in GIF.

günther

[MoshiurRashid]

As my assumption and as @g-andresen showed here, you had 4 corners open here.

In addition,

I want to explain how @g-andresen solved this. When you convert the dxf to fusion sketch, some of the corners doesn't connects with each other. (they have same end points but not connected). They are showed in white dot.

So what he did, he took the "coincident" constrain and selected the 4 corners in Left to Right box selection. That selection only selects the complete entity under it. So, the only complete entity under it was the points (line and arc is not completely in the selection so they were not selected). That's how Guenther selected 2 points standing on same place easily and make them coincident and connected! The closed geometry is formed!

I hope you understood. Let us know if you have more questions. 

[Anonymous]

Thank you @g-andresen and @MoshiurRashid I knew it would be something simple but for the life of me I couldn't figure it out!

[Tim.vanlaer]

Hi,  i also have a problem when insert a dxf in can extrude this. But when i move it to the correct position it doesn't extrude anymore.

Could anyone help me?

Regards Tim 

[g-andresen]

Hi,

The problem is caused by double vectors (superimposed lines).
Fusion "analyzes" the sketch in terms of closed line segments, which ultimately result in an extrudable profile.
If lines lie on top of each other, it can happen that several open polylines are detected, which do not form a profile.
In the screencast I demonstrate how to identify and remove such duplicates.

However, I have not removed all duplicates in the attached DXF, but would recommend that you complete the process with the source file itself.

günther

[Tim.vanlaer]

Hi ,

Thanks a lot, this works perfectly for me.

Regards Tim