centralize a rectangle to UCS

[reggy]

Will someone here please help a group ofbeginners?


We are using v 2007 and would like to know the procedure and also the proper sequence needed to centralize a rectangle to the Origin.


We have concluded that we need to use the line tool to draw a diagonal line, which gives us the center point, we don't know what to do thereafter.We have been told that the newer versions have a tool to do just this, which of course does not help us out using this out of date software.


Thanking you in advance, all seven of us.


Reggy

 

[Mihail]

One way:
Sketch a point. Place it in the UCS origin: P(0,0). Right click the diagonal then SELECT MIDPOINT. Press CTRL then select the P point. Make this points COINCIDENT.
Good luck !

 

[reggy]

Thank you so much!

 

[bdzin]

You should use the CENTER RECTANGLE sketch tool. When you extrude your part use the MID PLANE option. That will give you a perfectly centered rectangle. You could mirror top to bottom, right to left and front to back very easily.

Added Sept 8, 2012

If you use a CENTER RECTANGLE sketch tool on a plane and do a MID PLANE extrusion you do have an exactly centered extrude on the origin. I stated that mirror features could be easily used after that as the standard planes could be used.

I'm not changing my original post, I'm just clarifying it.


Edited by: bdzin

 

[reggy]

Thank you as well!

 

[Mihail]

Yes. As BDZIN say this can be done using mirror feature. But...

Every item in a sketch, every relation, every feature in a part, every mate in an assembly and so on, need resources to be computed.
So, as an advice, keep things as simple as possible. BDZIN's solution is an working one but need more resources than a simple rectangle with a diagonal.

By the way, even my first solution is a little bit more complicated: it is no need to sketch the point and place it at (0,0).
Simple select the diagonal's midpoint then, using CTRL, select the ORIGIN (in the FEATURE TREE MANAGER) then make this points COINCIDENT. This way the sketch will be simplified with a point.

 

[mjcole_ptc]

You can make a rectangle and add center points to each side H and V
lines then align these to your model origin or another arc or circle
center in your sketch. I don't believe 2007 had a center rectangle but
you can make a saved feature containing a rectangle as described. The
Center rectangle in sw2008+ contains two diagonals 1 more than
necessary. I usually delete 1 for cleanliness.

When I used
SolidWorks 2007 it was the Personal Edition and although later editions
will sometimes open these restricted files cause it can't figure out
they weren't made on the Professional version it won't help you for
2007. I wasn't as good at SolidWorks when using the 2007 and remember
the many workarounds I had to use because of inferior functionality in
the pre 2008 versions.

Not sure if this was possible in 2007 but
you may be able to use the Add Relations icons found in
Dimensions/Relations in the Commands window of Tools>Customize it
looks like a _|_ perpendicular symbol. now it is possible to Right Click
on a Line and choose select midpoint. There were a few bugs related to
this option not always appearing or only having it appear on the first
or second selection. If you choose Add Relations first and see a
collection box in the Feature manager you do not need to hold the CTRL
key to select multiple items. If you are using object-action and select
the items first you need to hold down the ctrl key to select multiple
items and based on what you select you'll see the available constraints.
Horizontal and Vertical relations can act on lines or between 2 or more
points.

http://help.solidworks.com/2010/English/SolidWorks/sldworks/ LegacyHelp/Sldworks/SW_Sketch/Sketch_Relations.htm

SolidWorks has moved all the help since 2009 online but most of it is still the same.
but don't expect everything in 2010 help to exist in 2007. For 2007 it's still in a html help file .chm
C:\Program
Files\SolidWorks\lang\english\sldworks.chm or the closest to that path
in your SolidWorks or "SolidWorks 2007" directory

Michael




Edited by: mjcole_ptc