Can't get a cut through in inventor 2023
I have created a car body inside of a ipt file. I am trying to make a hole through a lofted part however it does not work. Creating a normal extrustion works but not the cut. When i try to cut it the sketch disappears and i get a notification saying that it did not change the amount of faces.
If anyone have any solutions or reasons behind the problem please share.
All help appreciated!
3 Answers
It looks as though you have created features with sketches using a lot of projected geometry. That's normal practice. But then maybe you deleted the previous features that had the projected geometry. I can't tell which particular extrusion has a problem. When I first open the part, you have at least 9 sick sketches and features. As I started fixing the first broken sketch by just deleting the projected geometry it resulted in many more broken sketches further down the feature tree. This model has some significant problems.
You need to be very careful what geometry you project into a sketch. Edits to the original geometry can permanently break subsequent sketches. Oftentimes I will start with a main layout sketch that has the main details that will be projected into subsequent sketches. But the main layout sketch itself will not be consumed by any feature. Nor will I ever delete any geometry from it for any reason. I may also create various workplanes at key locations that will be use to locate sketches or be projected into sketches. All these things will be located at or near the top of the feature tree and will be independent of other features so they don't break due to other edits.
This is a particularly complicated part to make out of a single solid. I would suggest breaking it down into simpler individual solids that are then combined together. Or even better, Create simple individual parts that are then placed into an assembly.
The real problem seems to be features "DeleteFace19" and "DeleteFace20".
They turn the front cowling area into a solid with no interior volume. As if it was a surface model only. Then when you attempt to extrude Sketch210 as a cut, since the front cowling has no solid volume, you get the error that it had no effect on the part.
Suppressing "DeleteFace19" and "DeleteFace20" allows Sketch210 to be cut through the part. However this results in many surfacing operations being orphaned. So the DeleteFace operations need to be corrected.
I see nothing on this model that required the use of any surfacing operations. So most of the times you used the deleteface command were unnecessary.
Its a bit laggy but here is the finished video!
Thank you for the help
