Autodesk Inventor Users

Thank you for your advice. For this case, I like to have all the geometry in one sketch. I know I can deselect holding Ctrl on Wall ''B'' but does not work.

I doing how you show. Extrude does pick up both geometry. if I try to deselect one geometry and the inventor does deselect both.

If somebody has time to test, please download IPT and try to extrude in two different solids.

thank you.

https://grabcad.com/library/extruding-geometry-problems-1

You can't extrude 2 different solids from the same sketch unless the 2 solids are extruded from closed geometries that are physically "apart", i.e their lines have a space inbetween.

If you are using a dependent lines, Inventor Automatically will pick both, you have to make construction line the B ones, then into the another sketch using projection you can extrude B.

I had this Problem as well for many years!

What works for me is splitting the line of B where it meets with the lines for A. If the lines then are on top of each other you can delete one, or make it to a construction Line.

In hindsight it makes kinda sense, since Inventor isn't sure where the contour stops.

If you use lines with parameters you can leave the measurements, or convert the original line to a construction line.

Hope this works for you as well!

I can't open your file because I have only V2018 but I think the problem is that you use the line from wall B also for wall A. In this case just add points on your line intersections to make virtuell brakes of the line.

This is typical problem when you draw sketch separate lines or another reason is when you draw rectangular shapes so that you snap it some other rectangular points. I avoid Point to point constrains because if you had three lines connected same points then visually 2 have conection but one maybe have not. For extrusion you need to have mathematicaly closed boundary but visually is very hard to understand what line endpoint is accutally connected another line when you snap only one rectangular corner. To avoid this problem always draw rectangular shape so you will leave gap between another rectangular shape. Then you are sure you have closed loop. Then Connect rectangulars shape using horisontal or vertical or aligned constrain. Example- you need to create emty box 4 separate solid sidewalls and 1 separate bottom. Many users start sketch to draw outside rectangular shape and then make wall thickness offset and draw wall separation lines. This is tottaly wrong way. After first extrude you can not select another wall because first extrude used connected closed loop points. To make it right way draw one bottom rectangular shape in centre point and then draw 4 separate rectangular sides and leave small distance between bottom rectangular shape. Then use aligned line constrain and conect sides to bottom and eatchother. when you finish sketch Right click and share sketch and then you can make 5 separate extrusion for 5 separate solids

As mentioned in the thread you need to change the connecting (B) lines to construction lines.

That typical problem or issue is common sometimes. All the proposed solutions above are valid if carefully we can select what we want to extrude.

Multibodys is a way, One sketch several solids to be driven!

Construction geometry is another way however can be tricky because at the point of contact we can end we several overlayed lines which is, in my opinion not good.

When I normally do walls, I use rectangles, no matter how long, thick or wide, dimensional constraints will define wall dims, thickness etc, and CO LINEAR geometric constraints will put the walls in line one with respect the others. The rectangles will contain the solid, very defined by its boundaries with no errors allowing select/deselect functionality.

Hope this help