Half section of a simple turned part

Good day all,
I am pretty sure that there is a simple answer to this question but I
cant seem to figure it out.

I have a simple lathed part that I would like to section. However I
only want to see a section through half the part cutting through the
wall toward the centerline, but not right through the entire part.
When I do a standard section, and cut through the whole thing the
profile is duplicated, and it is cluttering up the drawing. I really
only want to see only one of the profiles and not both. Then I would
like to dimension this to the centerline, even though the centerline
is not in the sectioned view. Did any of that make sense?

If anyone knows how to do this I would really appreciate it,

Thanks,

Andy Kveps,

 

If I understand this,.. what you can do is create a section
configuration in the part file, this is, create a cut which shows what
you want per the view.
In the drawing you will have to assign (right mouse click over view or
in feature manager) the configuration per that projected view.
You can manually assign a cross hatch pattern to your cut face(s).

...

 

you could crop the view by drawing a box around the part you don't want
and then selecting crop view./

or if you havew a parent view on the drawing which is adding more
clutter you could do a partial section, either by drawing a line from
the center out, and answering Yes to the partial section view. you could
also draw two lines ar right angles that intersect at the axis of the part.

Or you could use the JB method where you just white out the screen where
you want to get rid of the lines.

Daisy.

 

I'll tell you what I do:

1)Create a section view,
2)Drag a rectangular drawing box over it, making sure that one edge is
aligned to the centre line or just beyond (sometimes clarifies the
view to be able to see the centre line in context),
3)Select 'Insert /Drawing view/ Crop. This will crop the view to your
box,
4)Dimension part as desired. I forget but you might need to draw in a
centre line to dimension to.

Having said that, I prefer to dimension turned parts as diameters as
otherwise, if you dimension parts as radii (to the centre line) you
really need to halve the tolerances. This often leaves you with
ridiculously tight tolerances on the drawing even if to measure the
part the operator then doubles the rad and tolerance anyway.

I generally show as diameters: Select the far point you want to
dimension and drag the dimension over the centre line to get it to
show as a 'diameter'. It may not have the diameter symbol at this
time. Then double click the dimension to obtain the Dimension
properties box. Select 'Display' and delete either the first or second
display and extension lines to suit. (Trial and error 1st time).Click
ok and then in the properties tab select 'Modify text' and add the
Diameter symbol to the dimension.

Sounds tricky but it's not once you have done it a couple of times.

Hope that helps.

Flynt

 

I have a simple lathed part that I would like to section. However I

This is a quite common approarch in some older drawings; the intention is to
save drawing space by dimensioning outer dimensions from the upper half and
inner dimensions from the lower half, or vice versa. Forget about crop,
Broken Out Section is your friend. Create 2 views, one showing your part
from the direction of the axis and a projection from the desired section
view. In the projected view, draw a rectangle which encloses half of your
part so that one line is collinear to the centerline. Select the 4 lines of
the rectangle and select Insert -> Drawing View -> Broken Out Section. To
define the depth of the section view, select the circular edge of the part
from the first drawing view. As a result, half of your part is sectioned to
the very center of the part. Insert model items to add dimensions.

Hope this helps!

-h-

 

Thanks for the help guys. I went with Flynts technique, but they all
would work for me.
Thanks again.