Creating a 'New View' and 'Saved View' in SolidWorks

When creating drawings from part or assembly files, often users need alternative view other than the standard views: Front, Right, Left, Back, Top, Bottom, Isometric and More Views: Dimetric, Trimetric. When creating a drawing with a file already open, the Current Model View checkbox is an available option.

          

One option is to position the model in the part file and use Current Model View for a drawing view. This is a snapshot of the graphic view of the part file used at the time of the drawing view creation. Another option is to create a Saved View.

Here’s how it works…Open the part or assembly file.  Here is a bracket shown in an ISO view. 

Create a view you would like to use for the detailed drawing.  For this example, I will pick the angled face and made the plane Normal To  .

 

 

To save this view, display the Orientation Dialog Box by doing one of the following:   

• Click View Orientation  (View toolbar).


• Click View > Modify > Orientation.


• Press the Space Bar.


• Right-click in a drawing sheet and select Zoom/Pan/Rotate > View Orientation.

The view will temporarily revert to the ISO view and display the Orientation window.

Pick the New View icon  .  The Named View dialog box will appear (note: the model will revert to the view to be saved.)  Enter the name for the new view in the View Name box.  Hit OK.

 

We have successfully created a Named View.  

Let’s take this one step further!

What if you want to use that same named view for other SolidWorks files?  When a custom view is created and saved, the view will be available within SolidWorks and available for every part or assembly model opened by the SolidWorks user.

To make a custom view available in all SolidWorks documents:

• In a SolidWorks document that contains a custom view, press the spacebar or click Orientation   (View toolbar). The Orientation dialog box appears.


• Hover over the custome view you want to make available in all SolidWorks documents. Options to save or delete the view appear.

• Click Save View to SolidWorks  .

 appears next to the view, indicating that it is available in all SolidWorks documents.

To access the saved view from another document, in the Orientation Dialog Box, mouse over Saved Views and select the view you want to add to the document.

 

To remove a saved view from a document, hover over the view name and click Remove View from Document .

 

To delete a saved view, in any SolidWorks document, in the Orientation Dialog Box, hover over Saved Views and click Delete View from SolidWorks.

To add the saved view to a drawing, add a drawing view and select the saved view that appears in the More Views area of the Orientation Dialog Box.

I hope you found this useful.

Thanks!

Judy Marlo

Application Engineer

Computer Aided Technology, Inc.

Exploded view alternate directions

When creating an exploded view in SolidWorks it is simple to move your parts in the local coordinate system along X, Y, and Z. What if you want to move a part in a different direction? In order to accomplish this we need to reorient the coordinate system. You will first select the component you want to move, then click in the box called z@(name of your assembly)

You will then select a new reference. In this example I am choosing the outer cylindrical surface of the part.

Notice how the reference triad has repositioned itself so Z is along the central axis of the cylinder. Just drag the blue error how you would normally move a component.

Another method to accomplish this is to use a sketch line instead of a component face. The sketch line can be 2d or 3d.

Thanks,

Jordan Nardick, CSWE
Applications Engineer
Computer Aided Technology, INC.

Rotate about scene floor

A brand new feature for SolidWorks 2013 is the option to rotate your model about a scene floor. This will lock the Y axis of your model vertically and keep your part file from flipping over. To access this feature right click anywhere in the view window and select rotate about scene floor.

Right button menu option turned on.

This image depicts four views of the same part file with the Y axis oriented up and down in each view.

Thanks,

Jordan Nardick, CSWE
Applications Engineer
Computer Aided Technology, Inc.

How to Use the New Orientation Dialog Box in SolidWorks 2013

Do you find yourself constantly changing views until you finally find the correct view that you wanted? Well, the Orientation dialog box received a nice new face lift for SolidWorks 2013 that you will find very useful. Simply press the spacebar or to bring up the Orientation dialog box, (or click the View Orientation button in the Heads-up View toolbar and click More Options, or pull down the View menu and pick Modify - Orientation.)

    

The new Orientation dialog box for SolidWorks 2013 now shares the same buttons for standard views as the Heads-up View toolbar. Another cool new feature in the Orientation dialog box is the View Selector.

The View Selector gives a very nice visual way to see the model views. If you have trouble visualizing what the right, left, front, back, top, or isometric views of your model will look like, this tool is a great enhancement for you. Click the View Selector button or press Ctrl + Spacebar to bring it up.

It is very simple to use. Simply highlight what view you want, either from the View Selector 3D box or even from the Orientation dialog box. If you hover over the button in the dialog box, a preview of that view appears and the corresponding faces dynamically highlight in the View Selector. When you select o view, the Orientation dialog box closes (unless it is pinned) and the model rotates to that view.

Another enhancement to the Orientation dialog box has to do with saving custom views. You can now create custom views and save them to SolidWorks, which allows you to reuse these saved views in different documents. after rotating you model to the desired view, click New View. Give the view a name and click OK.

    

The new named view now appears in the Orientation dialog box. This allows you to toggle between any of the standard views and this new custom view. This is not new to SolidWorks 2013. What is new is that next to this new named view is a Save View to SolidWorks button.

When you click Save View to SolidWorks, a globe icon appears in front of your named view. This indicates that it is now a global view that is now available in other SolidWorks documents. Simply open a different document. Click Saved Views in the Orientation dialog box and click the saved view(s) of your choice. One thing to note is that if you only click the check box, and not the view name itself, the named view is added to to the list of saved views, but the model does not actually rotate to the selected view.

Try it out yourself and see if the new Orientation dialog box, the View Selector, and Save View to SolidWorks will help improve your workflow. SolidWorks 2013 has many great enhancements that will continue to help improve the productivity of SolidWorks users around the world.

Neil Bucalo
Technical Analyst

Computer Aided Technology, Inc.

When creating a SolidWorks sheet metal flat pattern drawing view, why is the view not flattened?

Even though SolidWorks has greatly enhanced the sheet metal tools, we still get the question asked: When creating a flat pattern drawing view, why is the view is not flattened? To understand this better, let's go through the steps of what is suppose to happen when you create a new SolidWorks sheet metal flattened view.

1. Create a drawing from a SolidWorks sheet metal part document.
2. Insert the flat pattern view.

3. Right Click on the new drawing view and pick Properties. As you can see in the Drawing View Properties dialog box, SolidWorks automatically creates a configuration name DefaultSM-FLAT-PATTERN and sets the drawing view to use this named configuration.

This is what may be confusing to some. Since SolidWorks automatically creates this new configruation in the part document, whatever is shown in the DefaultSM-FLAT-PATTERN configuration is what will be shown in the drawing. Just because the name of the configuration says FLAT-PATTERN does not mean that SolidWorks knows to stay that way. A lot of the times, the DefaultSM-FLAT-PATTERN configuration is not in the flattened state. This can easily be done if the user does not realize what configuration is active. A quick example:

1. Switch over to the part document.
2. Set the active configuration to DefaultSM-FLAT-PATTERN.
3. Click the Flatten button in the Sheet Metal toolbar so that the part bends back up.
4. Switch back to the drawing. As you can see, the view is still set to the Flat pattern Orientation in the Drawing View PropertyManager, but the drawing view is no longer flattened.

So far, this has resolved the issue most of time by making sure that the DefaultSM-FLAT-PATTERN configuration of the part document is in the flattened state. I did have one other issue where the user's document template already had the DefaultSM-FLAT-PATTERN configuration. So, when the drawing view was inserted, SolidWorks could not automatically create the configuration and set the sheet metal state to flattened. The solution was to open a new part document, delete the DefaultSM-FLAT-PATTERN configuration, and resave the document template. The next time the user created a sheet metal part and then created the flattened drawing view, it worked correctly.

Neil Bucalo
Technical Analyst
Computer Aided Technology, Inc.