feature rebuilds only after double clicking the rebuild button..........how peculiar!

In short:
I've got a part wich has a sketch feature wich is dependant on an equation
which is dependant on a parent feature and a "grandparent" feature. When i
change the dimension of the grandparent feature and press the rebuild
button, only the parent feature updates but not the child feature! if i
press the rebuild button consequently again, then also the final child
feature (the sketch) updates, as it had to in the first place from the first
rebuild button-hit! did anyone encountered such persistant situations where
features refuses to update from the first rebuild button-hit, but "agrees"
to update after second rebuild attempt?

My specs are SW 2007 x64 sp2.1, Windows XP x64 SP1, 2GB RAM, AMD Athlon X2
4600 CPU.

In long:

If any one is interested in recreating this then do as follows:

1. sketch a rectangle.
2. boss/base extrude it
3. enter variable fillet on one edge of the resultant box
4. sketch on both perpendicular face to fillet face a line coincident from
each pair of fillet vertexs (two sketches: one on each face - bot sketcheses
are on parallel faces to each other)
5. create a loft surface using the two previous sketches an profiles, and
the tangent edges of the variable fillet as guide curves.
6. use replace face feature to replace the new surface with the varible
fillet face.

Now you have a variable chamfar as Anna Wood explained in her previous
response to Phil Evans (thanks!

7. create a sketch of a construction line on the "variable chamfer" face
between the two midpoints of two opposing edges and give it a driven
dimension. in the middle of the construction line create a circle and give
it a driving dimension.
8. insert equation: "circle diameter" = "construction line" / 2
9. create from the previuos sketch a cut feature.


Now: if you change one of the radius dimensions of the variable fillet and
hit the rebuild button then the "variable chamfer" will change
accordingly........but the hole (circular cut feature) will not chage with
it! only if you hit the rebuild button again then the cut fature will update
accordingly!

I dont know why solidworks acts like this, and i find it strange unless
there is something i'm unaware of driven dimensions and their use in
equations. i would love to read your insights or to get confirmation to this
issue from other users.

Thanks,
Gil

 

Hello Gil,

This is the default behaviour. Depending on your "stack", Solidworks
can only rebuild one at a time. Especially with equations.
Really depends on how you build your part.

Elmar

 

hmmm........strange but untill today, i was used to the fact that one
rebuild button-hit, rebuilds everything there is to update in a file, so
what you say comes as a surprise to me!
I made some further experiments regarding this issue and found something
else: If i click the rebuild on the toolbar as i'm used to, then there is
the need to click twice in order that SW will rebuild completly versus using
the ctrl + B keyboard shortcut which rebuilds everything at once completly
as it should (at least it should to my point of view).
When i turn to Tools>Customize>Keyboard then Ctrl + B is assigned to the
Rebuild command which i interptate as meaning the following (please correct
me if i'm wrong): "Ctrl + B" keboard button hit = clicking with the mouse
cursor on the rebuild icon in the standard toolbar! or isn't
it?.........strange......

 

Hello Larry,

The behaviour you have seen is dependent on how you use equations.
You CAN create features/sketches in combination with equations that
lead to what you have seen. Solidworks has two rebuild functions.

Rebuild the model
Ctrl+B

Force rebuild the model and rebuild all of its features
Ctrl+Q

See the help menu for further explaination. If you use equations that
use dimensions of a sketch as input value, then you can encounter
this effect. Solidworks first updates the sketch. Another rebuild will
then update the equation....

In a nutshell, if you don/t want the double rebuild - use excel
instead
to make your calculations. This is will update in one run and also
has the advantage of easier handling.

Elmar

 

Actually, a calculation like what he was talking about (dividing by 2)
would be best handled geometrically. Use construction geometry and
sketch relations to calculate the size without using equations or Excel
at all.

Putting a driven dimension on the left side of an equation causes
equations to need to be solved twice.

 

Actually, a calculation like what he was talking about (dividing by 2)

O.K. Matt......thanks for clearing this point to me. I was suspecting
somthing in the use of driven dimensions inside an equation is the main
culprit, because the warning massage i've got while doing so from solidworks
(i just wasn't sure of it).

 

Thanks for the explanation, Elmo. Because my model normaly contain only
small assemblies if any (many times i only do parts and drawings), and
because my workstation is pretty powerful for my work, i think i will stick
from now on to the Ctrl + Q keyboard combination.