sketch won't cut

[Anonymous]

Please take a look at this part. Sketch 6 won't cut leaving ribs like those show in the pdf file. Don't modify it because I'm using Inventor 2019. Just tell me what I'm doing wrong.

[SteveMDennis]

@Anonymous 

What do you mean it won't cut? What exactly are you trying and seeing as a result?

I did the following (albeit in an internal build not 2019 but I see nothing that I would not expect to work in 2019)

1. Turn on the sketch visibility (can't see it because it's in the middle of the blank.
2. Run extrude command
3. Window select all the profiles
4. Do a two way cut

The end result looks just like your PDF drawing in 3D...

[JDMather]

Did you set Midplane Through All?

I noticed that your first sketch is not fully defined - I would have recommended that you stop there and ask questions.

Then I noticed that you patterned Sketch6.  In general it is usually advisable to pattern features rather than sketch elements.

It might be useful in the future to create a Screencast Recording of your steps.

[Anonymous]

How do I set midplane through all?

[SteveMDennis · Accepted solution]

in the 2019 dialog, midplane is the 3rd button in the extents area (with arrows going both ways)

Through all as JD points out is in the drop down also in the extents "All"

And choose the cut operation button, 3rd down in the vertical column.

[swalton · Accepted solution]

@SteveMDennis I agree.  I am using Inventor 2019.4.  I can use Sketch 11 to cut the openings in the wheel.  I can also use Sketch 6.   

@Anonymous if you edit the sketch, hit the F7 key to slice the graphics and then press E (the keyboard shortcut for the Extrude feature) you can select all the closed regions in your sketch.  I exit most of my sketches by pressing E for Extrude or R for Revolve.

Modeling Notes (feel free to ignore these if you want)

1. Fully constrain your sketches to the Origin workfeatures or other feature geometry.  Not doing so leads to pain and unexpected results at some point in the future.  The only time I don't fully constrain all my sketch geometry is if some part of the sketch will be adaptive in a parent assembly.  I project reference geometry from the origin workfeatures or existing features, draw the sketch geometry, add any sketch constraints that Inventor did not automatically apply, then add any dimensions to fully constrain the sketch.  Ideally, my sketch dimension scheme matches the drawing dimension scheme I plan to use.
2. Sketch 6 and Sketch 11 are the same, I think.  No need to have both in your final part.
3. Does Workplane4 add anything to your design? If not don't create it. You already have the XY plane at the center of the part.
4. Chamfers and rounds should be at the end of the model tree unless you need them as part of an earlier feature.  Move the EOP marker up and down the model tree as required to insert before and after other features.  I tend to model in a Big-To-Small order as I refine the part.  I also tend to group related features in the same section of the model tree.  I find that helps me understand the model after 2-3 years away from it.
5. I would normally model the rib cuts as two different feature patterns. One for the straight sections and a separate one for the wedge sections.
6. Use the obvious part symmetry about the origin workplanes if at all possible.