With all the new functionality with view labels in SolidWorks 2014, some ancillary enhancements have also come about as a result from customer feedback during Beta Testing. One of these enhancements has been the new capability to display any view’s angle within an annotation note. Why would anyone need something like this?
Well, there are four default options for the display of the angle symbol auxiliary views.
- Show rotation symbol with rotation angle
- Show rotation angle
- Show the text “ROTATION” followed by the rotation angle and direction
- Show just the angle
If your company chooses to display just the rotation angle (as is common for GOST drawings), it is still sometimes necessary to display the rotation angle. Because the view label is a global setting within the drawing, there’s no way to accomodate this deviation from the standard settings without having some hugely complicated user interface to track individual labels here and there. So, instead, one additional annotation tag has been added. The advantage is that this new tag is available for any drawing view (not just auxiliary and section views). The new tag is <VIEWANGLE>. Type this into any annotation note. As long as that note is a attached to a view, that view’s angle will be shown. As an example, this new tag can be added to the auxiliary view label after the <VLANGLE> tag (or anywhere else in the note).
The settings and the result of using the new tag:
Auxiliary view functionality has now been expanded to follow several international standards more closely. When an auxiliary view is created at a nonorthographic angle, the standards specify that the view should be rotated into an orthographic direction. To account for the change in alignment, ASME and GOST standards specify the addition of a rotation symbol that may also include the actual angle of rotation. SolidWorks now supports these requirements.
To set an auxiliary view to orthographic rotation for the example above:
- Right-click on the auxiliary drawing view.
- Select Align Drawing View, then Horizontal to Sheet Counterclockwise.
Select Align Drawing View and rotation direction
The view is rotated. Angle symbol and degrees is added to the view label
If center marks are in the view, they can be rotated by selecting them and entering o (zero) in the Angle group box in their PropertyManager.
The display of the angle can be adjusted in the Document Properties under Tools>Options…>Document Properties>Views>Auxiliary in the Label options area.
These options and capabilities are also available for Section Views with the same instructions as above.
Also, these options are available regardless to standards. However, GOST standard does has special symbols. All rotation symbols are also available in the new Views symbol library category.
The next article in this series will cover how to add a view’s angle of rotation to any view type.
A big leap forward for the Hole Wizard in SolidWorks 2014 is the support of slots as features! I’ll say this another way. You can now create slots with Hole Wizard!
When SolidWorks first announced that there was going to be support for slots many years ago, I was a tad bit disappointed when I found out how. Slots were only available as sketch elements. Although I did find this useful and it did streamline my workflows, I found it to be a step short. I was still having to make slots as separate extrude-cut features. Converting holes to slots and slots to holes still needed a rather lengthy workaround.
SolidWorks 2014 addresses this, and how! Slots are now supported by the Hole Wizard in spades.
Slots with counterbores, slots with countersinks and slots with..umm, well, straight slots with no counter-anything.
Not just that, you can quickly switch between slots and holes, based on design needs for your particular phase of development.
Holes become slots with a quick edit (and then back again, if you wish)
On Drawings, view labels are special annotation notes that are attached to views such as Detail, Section and Auxiliary. Previous versions of SolidWorks tightly controlled these labels via the Document Properties (Tools>Options…>Document Properties tab>Views Labels). When changes were made to view labels in the Document Properties, those changes were then forced onto all view labels of that type throughout the drawing. Sometimes you might want to add specific information to a particular view. SolidWorks often reverted manual edits to the view label. The settings within the Document Properties were enforced to the exclusion of other edits. There is a setting that allows you to override this behavior called “Manual view label” in the view label’s PropertyManager. The drawback of this setting is that elements within the view label all become simple text and no longer update (e.g., if the scale of the view was changed, the view label would not automatically reflect the change).
Edit View Labels in SolidWorks 2014
SolidWorks 2014 introduces sweeping improvements to view labels. First, a new setting is now available in the view label’s PropertyManager called “Use document layout”. When this is checked, the Document Properties prevail. When this is unchecked, you can manually edit the layout of the view label while still maintain the values for scale, view letter, name, etc. This means, you can type your own text in-between or even on a separate row of text.
Using tags for view label elements
The second improvement actually makes the first improvement possible. View elements such as scale, view letter and name are now represented by tags. These tags are viewable when editing the view label within the Edit Text Window.
Didn’t know that there was an “Edit Text Window”? It’s always been there. Right-click on any annotation note and choose “Edit Text in Window”. This dialog has been expanded for view labels.
As shown in the above image, buttons are now included that allow you to add view label elements. The dialog is smart enough to know when elements are already included in the edit box or when the elements are not valid for a particular view.
You might notice that these buttons are also available when editing the view label directly in the graphics area too.
Labelling views with angles (to be cont’d…)
In addition to all of the above enhancements, SolidWorks 2014 now has a tag that allows you to add a view’s angle of rotation. However, more on that in a future article. A lot more.
For drafters that need more control over how dimensions are displayed on their drawings, SolidWorks 2014 has introduced a couple of new controls. First, styles for extension lines and dimension lines can now be assigned independently from each other on dimensions. The default line styles can be set in Document Properties for each dimension type, and within the Dimension PropertyManager.
In the PropertyManager, a new group box has been added, called “Extension Line Style”. Within this group box, there is an option to keep the line style that same as the leader/dimension style with the option “Same as leader style”. If you wish to use the document defaults, selected “Use document display”.
If both of these settings are unchecked, you can set the extension line for the selected dimensions separately from the dimension line style. The example here shows the line thickness as different.
Second, you can now set individual extension lines to display as centerlines. This allow you to identify extension lines that emanate from holes, per ASME practices. To make this change, right-click on the extension line and select “Set Extension Line as Centerline”.
To change it back to normal style, right-click on the extension line again and select “Reset Extension Line Style”.