From SolidWorks Blog:
In SolidWorks 2013, The Auto Route tool includes an option to create a route based on existing geometry. To route along geometry, specify a start point, one or more planar faces, and an endpoint in the Auto Route PropertyManager. Routing automatically creates a route from the start point to the end point that runs parallel to the faces. You can specify the distance between the route and each planar face.
From the SolidWorks Blog,
SolidWorks 2013 won’t be officially unveiled until September 10, but over the next few weeks, we’ll be giving you sneak peeks at a few of the new features we’ll be shipping this fall. And here’s the first.
In SolidWorks 2013, center of mass is a selectable entity in drawings, and you can reference it to create dimensions. In a drawing, you can create reference dimensions between center of mass points and geometric entities, such as points and edges.
Every once in awhile in drafting, you just need an arrow, with no text, attachments or any other extras. Maybe you need to specify air flow, grain direction, inspection queue, assembly instructions, or one of a hundred other reasons. How do you make just an arrow in SolidWorks? Answer: Multi-jog Leader annotation tool.
Mutli-jog Leader is an oft overlooked tool that pretty much lets you make whatever arrow configuration you like using the same leader style of notes.
To make a simple leader with no text, start the Multi-jog Leader and select your first point. One arrow will point to the location where you clicked. The other end of the leader will follow the mouse cursor. Choose a second location and double-click to complete your leader. This will add another arrow directly opposite your first arrow.
Get rid of one of the arrows by RMB clicking on the tip of the undesired arrow and choosing the arrowless option.
Here’s what you end up with.
You can adjust the other end to be bigger (by RMB clicking on it and selecting Size…). In the case of the example below, I’m using the arrow to represent fluid direction of a flow body.
There is a number of good articles that have popped up recently in the SolidWorks blogospere. Here is a selected set of particularly interesting finds:
Enjoy!
**OUTDATED Content: Update–>SOLIDWORKS 2020 now allows you to add Geometric Tolerance and Surface Finish symbols onto your Sheet Formats directly without the following workaround**
SolidWorks Sheet Formats do not support Geometric Tolerance frames. So, what can be done if you wish to display a frame with your Sheet Format on drawings?
First, a quick review. SolidWorks has two separate files that serve as the starting point for creating new drawings. The primary file is the Drawing Template (*.slddot). Every time you start a new drawing, it must be from an existing Drawing Template. The template contains all the settings and other information needed for every drawing. In particular, it uses information from a Sheet Format (*.slddrt) for the border and title block. Each time you create a new sheet on your drawing, the Sheet Format is directly loaded. However, neither the Sheet Format or the Drawing Template automatically update existing drawings. For more information on Sheet Formats and Drawing Templates, see SolidWorks Help. The tip found in this article is for more advanced users and CAD Administrators that are already familiar with these topics.
Back to the story. Perhaps your company is moving towards using the model to define your product, but still uses the drawing to established specifications, such as tolerances, general notes, process control dimensions, etc. Common practice for this scenario is to establish a generic Profile specification on the drawing that is then applied to the model. But, you cannot store a Geometric Tolerance frame within a Sheet Format. You won’t likely want to draw your frame using sketches.
Solution? You can have a Sheet Format display a Geometric Tolerance frame that is present on a Drawing Template! Here’s how.
1. First, make backup copies of your Sheet Formats and Drawing Templates! OK, once that is done, open your Drawing Template using File>Open dialog set to Template (*.prtdot; *.asmdot; *.drwdot)
2. Create your Geometric Tolerance frame using the Geometric Tolerance annotation tool.
3. Place your new frame in the lower right corner of your Drawing Template. Don’t be concerned if it overlaps the border, but it is a good idea to keep it inside the paper space.
4. Create an annotation note (Insert>Annotations>Note…) and place it anywhere on the drawing.
5. While the annotation note is still being edited, click on the Geometric Tolerance frame. The frame will now appear in the note. Select OK to accept.
6. Select the new note.
7. Press CTRL-X. The note should disappear, as it is being cut from the Drawing Template.
8. RMB click on any empty area of the blank paper space and select Edit Sheet Format. This will take you into the Sheet Format editing mode.
9. Click on the approximate location where you wish the frame to appear and press CTRL-V. This will insert the note onto the Sheet Format. Click and drag it to the desired location.
10. RMB click on an empty area of the paper space. Select Edit Sheet. This will exit the Sheet Format mode and return you to normal drawing mode.
11. RMB click on the original Geometric Tolerance frame and select Hide.
12. Goto File>Save to save your Drawing Template.
13. Goto File>Save Sheet Format to save your Sheet Format.
(14.) Now, if you wish to edit the frame later, simply use View>Hide/Show Annotations. The hidden frame will appear faded gray. Select it and it will turn black. Press ESC to exit the Hide/Show mode. Edit the frame as your normally would any Geometric Tolerance frame. When done, hide it again. You may need to Rebuild to see the update.
Note: If you open the Sheet Format directly without loading the Drawing Template or if you load the Sheet Format into a drawing created with an older Template, the annotation note containing the frame will be blank. This is because the information is contained in your new Drawing Template, but the note is in the Sheet Format.
Remember this old faithful interface for creating Geometric Tolerance frames (a.k.a, GD&T feature control frames, or GTOL annotations)?
There a new thread on the Drawings forum at SolidWorks Forums asking about how you use this user interface to create Geometric Tolerance Frames. Your input is very welcome there (and here, if you wish). What would you do to improve the inferface?
