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Inventor is not ultra flexible to extrude anything you throw at it, if there are too many inconsistencies. Your best bet is to fix these issues in AutoCAD before you introduce the profiles into a sketch in Inventor. For example, look at this one, which looks fine at a distance, but up close is garbage:
In AutoCAD a couple of the tools I've used before for this were:
1) Select your polylines/curves and type "PE", then pick "Decurve", if most of the lines should be straight anyways;
2) Zoom into corners like the one above to fix them manually, or use the command "PEDIT" > "M" (for multiple) > JOIN > JOINTYPE > BOTH > "1.0" (fuzz distance), then trim any flying edges resultant from this.
3) Try importing from AutoCAD into Inventor by simply "copying to clipboard" those profiles and then right-click "Paste" in an Inventor sketch.
I hope this helps you figure it out on your own. Best of luck.
Inventor is not ultra flexible to extrude anything you throw at it, if there are too many inconsistencies. Your best bet is to fix these issues in AutoCAD before you introduce the profiles into a sketch in Inventor. For example, look at this one, which looks fine at a distance, but up close is garbage:
In AutoCAD a couple of the tools I've used before for this were:
1) Select your polylines/curves and type "PE", then pick "Decurve", if most of the lines should be straight anyways;
2) Zoom into corners like the one above to fix them manually, or use the command "PEDIT" > "M" (for multiple) > JOIN > JOINTYPE > BOTH > "1.0" (fuzz distance), then trim any flying edges resultant from this.
3) Try importing from AutoCAD into Inventor by simply "copying to clipboard" those profiles and then right-click "Paste" in an Inventor sketch.
I hope this helps you figure it out on your own. Best of luck.
Hi! The sketch is a bit far away from the origin. To make your life easier, move the sketch geometry closer to the origin. When Extrude does not work, it usually means either the profile is leaky (having tiny gaps or drastic curvature change) or there is an Inventor bug. The quickest workaround is to use Boundary Patch command to create a planar trimmed surface. Then use Thicken command to create a solid body. BP was designed to tolerate leaky profiles like this.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Hi! The sketch is a bit far away from the origin. To make your life easier, move the sketch geometry closer to the origin. When Extrude does not work, it usually means either the profile is leaky (having tiny gaps or drastic curvature change) or there is an Inventor bug. The quickest workaround is to use Boundary Patch command to create a planar trimmed surface. Then use Thicken command to create a solid body. BP was designed to tolerate leaky profiles like this.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Hi Johnson, I've played with it earlier, but only partly success.
Boundary patches can be done with 4 upper regions, but not with the lower regions.
One of the sketches turned pink, additionally. I couldn't repair it.
Walter Holzwarth
Hi Johnson, I've played with it earlier, but only partly success.
Boundary patches can be done with 4 upper regions, but not with the lower regions.
One of the sketches turned pink, additionally. I couldn't repair it.
Walter Holzwarth
Hi! The seemingly simple curves actually are quite complicated. Some of them are self-intersecting. I suggest you use SPLINEDIT command in AutoCAD to convert it to a PLINE. Then import it to Inventor.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Hi! The seemingly simple curves actually are quite complicated. Some of them are self-intersecting. I suggest you use SPLINEDIT command in AutoCAD to convert it to a PLINE. Then import it to Inventor.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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