V shape cut out??

[pyromech]

How would you cut those two indents (vshape) along the wall?

I am not sure if a sweep profile along the wall will do because the wall has different angles unless I sweep along a curve. Is that a Vshape cut? doesnt look like from the top

 

[pyromech]

Anyone, here is pro/e file

 

[jeff4136]

There are a couple of things you can do as a courtesy
when posting models.
1) Make known the generating software version.
2) Suppress all features and save as *.zip.

> unless I sweep along a curve.

That's what I would probably do.

> Is that a Vshape cut? doesnt look like from the top

That's a 2D drafting sofware generated drawing and
details like that are going to convey the general idea
(sometimes true of b-rep models, too).

Start with what you see, somehow determine intent /
function, consider manufacturing process and then do
what you can to model the geometry that would be created.

(Attachment: prt0001--wf2--.prt.zip, ~90 KB)

-Jeff Howard (wf2)
Sure it's true. I saw it on the internet.

 

[pyromech]

thanks for the redo.
My file was done in Pro/E W3.

The model looks extremely confusing, you have quilt, offset, extend, merge features which can be replaced with a revolve cylinder feature. Whats the purpose? Unless they were used to generate the surface sweep which only works on surfaces not solids???
I prefer to omit the surface revolve2 cut at the end of the keyway but it gives me a merge feature error. Can you please erase this?

If you look at my previous file, the solid sweep cut penetrates thru the wall. Look at the outside cylinder wall and you will see a sliver cut. Was this the reason for using surface cuts instead of solids?

thank you so much

 

[jeff4136]

> you have quilt, offset, extend, merge features which
> can be replaced with a revolve cylinder feature.

They can be replaced with a revolved feature that duplicates the offsets.


> Whats the purpose?

That quilt is just used, as reference, for creation of the 'v' sweep trajectory. Depending on intent, you could* probably omit that whole set of features and just go for the sketched trajectory using X sec Sketcher References to define offsets and tangent directions. I wasn't quite sure what that would look like and wanted to see what the deviation would be; conic arc to actual intersection curves.


> I prefer to omit the surface revolve2 cut at the end of
> the keyway but it gives me a merge feature error.
> Can you please erase this?

To understand the reason for the Merge failure if you omit the revolved cone section; create an intersection curve using the swept 'v' shape and the main body surfaces. You'll see that it makes an incomplete body trim boundary.

So, you can 'cap' the lower end of the swept 'v' with a planar Fill surf or Boundary Blend after deleting the revolved cone to restore the complete trim 'loop'.

You might also use another Sweep function that has a 'capped ends' option or, if you're working it as a 'solid' object, use solid / cut feature options.


> If you look at my previous file ...

I don't have the necessary upgrade to allow me to open WF3 files in WF2, so can not see your file.


> ... the solid sweep cut penetrates thru the wall. Look at
> the outside cylinder wall and you will see a sliver cut.

I can only guess that you are either seeing a graphics artifact (due to low resolution graphics settings?) or the sweep trajectory is improperly defined and is actually cutting through the outer body face.


> Was this the reason for using
> surface cuts instead of solids?

No. Using Solid features is usually quicker, more efficient. Using Surface features usually requires more user input, more steps, but allows a more flexible approach. Either way, in the end, the resulting b-rep geometry should be the same.

* There are several variations that ~could~ be used to define and create that feature depending on how accurately you want to represent some specific process.

-Jeff Howard (wf2)
Sure it's true. I saw it on the internet.

 

[willcambridge]

I didn't look at the proE file but the drw looks complicated. I would probably consider using several features to achieve the final result, rather than one or two highly complex features. This method might or might not mimic the manufacturing process; but it might be a quicker way to get a good CAD model, and easier to make changes, if you have a good sense of what your dependencies should be.

PS Was that a hand-made drawing?