Re-Assign Original Coordinate System in Assembly View 1

[vmuro]

I created an assembly and it turns out that I have assembled it in the incorrect views. My actual TOP view shoudl be my FRONT view. Is there an easy way to reset/re-assign the original coordinate system so that I can make my TOP view become my FRONT view? I don't want to go back and redo the mates for the planes, etc. Thanks in advance.

-VM

 

[CorBlimeyLimey]

Simple method ... Use the Orientation menu (spacebar) to re-assign the views.

http://help.solidworks.com/2010/Eng...p/Sldworks/Display/HIDD_SELECT_NAMED_VIEW.htm

To change the orientation of the standard model views in the Orientation dialog box:

1. In the Orientation dialog box, double-click one of the named views to select the new orientation. For example, if you want what is currently the Left view to become the front view, double-click Left.
2. Select the name of the standard view you want to assign to the current orientation of the model. For example, select Front if you want the current view to become the front.
3. Click Update Standard Views art\OR_UPDAT.gif. This updates all of the standard views so they are relative to the selected view.
4. Click Yes to confirm the update.

The downside to that method is that it can all too easily be reset to the default views.

 

[CorBlimeyLimey]

Better method (IMO);

Only mate the first part in the assy to the assy planes (or origin and axes). Then mate all other parts to the planes or features of the first part, or subsequent parts if they are more logically associated. Using this method allows all the parts to be re-oriented by simply re-assigning the grounding mates of the first part.

 

[vmuro]

Ahh...thanks for the tip. I used the first method to make my BACK view the new FRONT view and it work perfectly fine, except the coordinate system axes do not change (at the lower left of the screen). I was expecting them to re-orient themselves to x-> but rather x remained facing <-. Next time I will mate components per your second (and better) method. Thanks for your help.

Another question for you: In a drawing view, if I create a sketch and dimensions it, then I choose to hide the dimensions, is there any way to show them again?

-VM

 

[CorBlimeyLimey]

View > Hide/Show Annotations
Select the "ghost" dimensions to be shown
Hit Enter

 

[TheTick]

Rename your views "X-Y", "Y-Z", and "Z-X", and stop worrying about it.

 

[vmuro]

Will do. Thanks for all of the help...

-VM