Help With Assembly Drawings

Hi everyone.

I am very new to using Solidworks and working on learning this new
software. I have been using AutoCAD 2002 LT and I am very impressed
by the capabilities of Solidworks.

After completing several parts drawings all drawn in the front plane I
am having trouble with front view of the assembly. The parts consist
of a flat plate, small hub shaft, bearing retainer plate, bearings and
some bolts.

After I have mated all the parts together using coincidents and
concentrics and all looks well when I have completed the assembly
except when I look at the front view, lines that should be vertical
are a little off vertical.

Any ideas on what I have done wrong? I think I might have something
to do with having to rotate bearings and bolts to line up with holes
prior to final mating of the parts???

Any input would be greatly appreciated.

Thanks.

Jimbo

 

When you inserted the first part did you just drag it in and drop it or
did you mate it to the assembly planes to get the orientation you
wanted. Chances are your first part is fixed at an odd angle.

 

I drag and dropped it and kept adding parts from there. Should I
"insert/ref geometry/plane" or try "insert/ref geometry/mate
reference"?

Thanks

 

It sounds like it could be one of a few things. First, check what Top
has indicated in the previous post. While in the assembly, insure that
your named views have not been reset to some skewed angle. If you find
that everything appears correct in the assembly, then proceed to open
the drawing. Now insure that the main drawing view is using a named
view (you may have selected "current view" when you placed this view
and it grabbed whatever view the model was currently at)...or you could
delete the existing views and place a new view and be sure to use a
named view.

 

Expand the tree for your initial part, select one of the planes from the
expanded tree. Then ctl-select the cooresponding plane from the assembly,
you can then rotate the assembly and see if the two planes are at least
visually the same orientation. Repeat for the other planes.
If they are not the same, right click your first inserted part ( should
have a (f) next to the name ) and select "float". Then select a plane from
that part and the same plane from the assembly. Mate them as coincident.
Repeat for the other two planes.
If that was your problem, you can avoid it in the future by ensuring
that, during your first part insertion into a new assembly, you have
"view-origins" enabled. When you are hovering with the first part attached
to your cursor ( preview ) and your cursor nears the assembly origin, the
part will snap to the origin. When you click, it will essentially mate all
3 planes and fix the first parts location ( no mates actually are inserted,
but that is the effect ).