CATI Tech Notes has an interesting SolidWorks trick for getting your custom properties to accept values with multiple lines:
Category: Tip/Trick
SolidWorks quick tips and tricks.
Revision Clouds: What else is new ( Tip/Trick )
As noted in a previous article, revision cloud is a new annotation in SolidWorks 2013. Well, here’s a little trick not mentioned in the What’s New that you can use on revision clouds once you’ve placed them on your drawing. Highlight the revision cloud and goto Tools pulldown>Sketch Tools>Rotate. The Rotate tool will allow you to rotate your revision cloud annotation.
Rectangular revision cloud just minding its own business.
Gah! Someone has started the Rotate tool and is rotating the revision cloud.
Well, the cloud was successfully rotated and just left there to highlight the change at its new angle.
New in SolidWorks 2013: Hide Section View Cutting Lines (not found in What’s New)
With all the drawing improvements in SolidWorks each year, there’s often some small ones that don’t make it into the What’s New file. Last year, I covered several small enhancments in SolidWorks 2012 that weren’t in the What’s New. Well, it’s now time to start covering SolidWorks 2013. I’ll cover some of the bigger enhancements for SolidWorks, but I’m also going to cover some of these hidden gems too.
Section views are made of several elements, including a parent view, a cutting line, labels, and the section view itself. Both ASME and ISO standards have situations where the cutting line is not shown, such as with half sections or when the cut is obvious. Prior to SolidWorks 2013, hiding the cutting line required workarounds. In SolidWorks 2013, there is a very simple command now available.
To hide a section view’s cutting line, RMB click on the either the cutting line or the section view. Select Hide Section Line. That’s it.
Of course, the question now is, how are the cutting lines unhidden once they are hiding? Easy, RMB click on the section view itself and click on Show Cutting Line command.
The cutting line returns to the parent view as though it never went away in the first place.
Pointy arrows without the ears (a.k.a, text)?
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.
How to add a Geometric Tolerance frame to your Sheet Format
**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.
Visually determine the depth of a Broken-out Section in a Drawing View during preview
Adding a broken-out section to a drawing view is very useful to show detail inside of a part without resorting to creating an additional Section View. The Broken-out Section tool in SolidWorks allows you to quickly add this detail to an existing drawing view by simply drawing a closed spline and establishing a depth. A preview option allows you to see the result of your choices. The drawing view updates in real time as you change depth.
However, sometimes, it is hard to visualize the depth while you are creating the broken-out section. Some users will simply step through various depths until the broken-out section looks about right. This trial and error method can be time consuming.
The Broken-Out Section tool is actually smarter than that! It detects when there are projection views of the current view (either parent or child). If there is a projection view, you can click on the specific feature you wish to slice with the broken-out section. To use this cool function:
- With the Broken-Out Section tool active and cut area established, click on the Depth Reference field in the PropertyManager.
- In the adjacent side view, you will see a yellow line that represents the current depth of the broken-out section cut. Click on the feature you wish to cut through. The depth line will shift to the center of that feature.
- Click OK to accept.
The above method may not always be feasible. Perhaps the detailed components are too large to show the multiple views on screen at the same time. Or, perhaps there is no feature that readily provides desireable results.
Here’s a trick that may help. Use 3D Drawing View tool to rotate the view in 3D. As you adjust the depth in the PropertyManager, the 3D view of the model will update accordingly.
1. With the target view highlighted, choose 3D Drawing View tool.
2. Rotate the view to a desirable angle.
3. In the PropertyManager, change the depth.
4. Select OK in the PropertyManager when desired depth is found. Then exit the 3D Drawing View tool.
The result is a happy broken-out section in your target drawing view.
