Category: Tip/Trick

SolidWorks quick tips and tricks.

HOW TO CHANGE/SWAP TEMPLATE/SYSTEM OPTIONS IN SOLIDWORKS

I have heard this request many times so putting it up over here. The whole credit for this should go to Stefan Berlitz of http://solidworks.cad.de/ http://swtools.cad.de . Without his wonderful macro, this option might not have been possible.

Before starting the process I will strongly advise you to make a backup of the files.

  1. Open you part, drawing or assembly file from which you want to copy the Tool, Options> System Options /Document Properties Settings.
  2. Open the Excel based macro and choose the tab based on type of you file.
  3. In the Excel sheet, click on Get Options. This will copy the Document Properties Settings for that particular file. Repeat same for System Options.
  4. Close the SW file.
  5. Now open you part, drawing or assembly file to which you want to copy these setting or overwrite their setting with these one.
  6. Go back to Excel sheet and click on Set Options for both System Options and Document Properties Settings.

Cool, enjoy with your new part, drawing or assembly file template.

Get the macro here: mac_copydoc.zip

Lot of thanks to Stefan Berlitz for sharing his macro. He has also explained how to use this macro in a much efficient way in the same excel file.

Dimensional limits related to an origin

In SolidWorks 2007 drawing mode, the ability to change the size of individual dimension arrows (so that they were different than the drawing) was limited to a tricky use of favorites.   Starting with SolidWorks 2008, that situation improved.   SolidWorks now allows the user to set the size for individual dimension arrows.  For me, using arrows of a different size from the drawing default was only required once in the past.  However, I recently had the need to use this function for dimensioning limits from an origin. This is a special kind of dimension where the tolerance of a dimension is set between two features but applied in only one direction.

From paragraph 2.6.1 of the ASME Y14.5M-1994 standard:

In certain cases, it is necessary to indicate that a dimension between two features shall originate from one of these features and not the other.  The high points of the surface indicated as the origin define a plane for measurement.  The dimensions related to the origin are taken from the plane or axis and define a zone within which other features must lie.

The origin of such a dimension is shown by replacing that arrow with a circle.

Meaning

This is where we get back to talking about SolidWorks.  You can change the shape and size of the arrows on one or both sides of a dimension.  The problem is that once the dimension arrow is changed to a circle, its size cannot be adjusted. This means that if the circle is too small (as it likely will be) the size must be changed to the arrow before switching it to a circle.

The following are the basic steps to establishing a dimensional limit related to an origin on a drawing in SolidWorks 2008 or higher.

Instructions 1 and 2

This following chart will then pop up at that location on your drawing view.

Pop up chart

3. Select Size, to bring up the next window.

Arrow size changing window

4. Deselect Use document arrow size and edit the arrow width.  Accept by choosing the OK button.

Enter width

No, you aren’t done yet.  There’s more.  Remember, earlier I said the situation was easier.  I didn’t say it was easy.

More steps

Again Again

7. Select the fifth item down on the pop up chart, which is the circle at the end of the dimension line.

Final Product

After all of this, you’ll finally have a dimension that establishes its tolerance from an origin per ASME Y14.5-1994 paragraph 2.6.1 and figure 2-5.

UPDATE: Newer releases of SOLIDWORKS will allow you to apply a size directly to the circle arrow. So, although the above instructions still will work, there are some extra steps that are no longer necessary.

Different ways to Mate with a SLOT -1

Now we have finished and learned the techniques of making a SLOT, the second question comes up in the mind is “How to Mate with a SLOT”. Again there can be several ways to achieve this and one may adopt the method which he/she finds easy and quick to use. In this chapter let’s discuss about various simple ways of mating with a SLOT.

To use these methods you need a simple plate with a Slot of any size, a cylindrical, rectangular or square part with diameter/width equal to or less than slot width. In this chapter I’m going to use the cylindrical part (pin). I will be covering another discussion on same topic with a square part too.

Start you assembly with the plate inserted as the base part and fixed. You can also use mating techniques to position your plate. Now insert you pin which you want to mate with the slot.

MS1

Method 1: With your assembly opened and both the part inserted, select the back face of the plate and bottom face of the pin. Add a coincident mate between them. You can select front and top faces too. This is to set the initial position. Now show on the temporary axis (View > Temporary axis) to display the temporary axis of the pin. Select the side face of the plate and the temporary axis of the pin and give a distance mate. Repeat this with the bottom face. Your pin is now in to the required position.

MS4

Method 2: Using the same technique as described in method 1, use the planes instead of the temporary axis of pin to give distance mates with the side and bottom faces of the plate. Your planes may vary from the one shown in the picture.

The difference in the above two methods is that in Method 1 the part is not fully define and its free to revolve on its axis whereas in Method 2, the part gets fully defined.

Method 3: This is a combination of above 2 methods. Add a distance mate using the side face of the plate with the corresponding plane of the pin. Now show up the temporary axis if they are not on. Select either of the temporary axes of the slot and corresponding plane of the pin. Add a coincident mate.

Method 4: If your slot width and diameter of the pin and equal then you can use this method. Add a tangent mate between the side face of the slot and the cylindrical face of the second part. Then add a distance mate with the bottom/side face depending upon the location of your slot with the corresponding plane/temporary axis of the pin.

or

Method 5: In this method, RMB on the edge of the plate and select “Midpoint”. Then select the corresponding plane of the pin and add a coincident mate. Then add a distance mate with the bottom/side face depending upon the location of your slot with the corresponding plane of the pin.

Method 6: This is tricky method and I prefer to use this method most of the time. Open the plate and edit the slot sketch. Add these two construction lines to your slot sketch. Now in assembly, select to show the slot sketch. Use the planes of the pin and mate them with the corresponding construction line

 

 

These are few of the methods which I use for mating with a slot. I would be interesting to hear if you more methods or any other method that you use for mating with the slot.

Using Empty Views (Part 2: How to use them)

My articles on Empty Views in SolidWorks have been long in coming.  This is not due to the topic being complex or anything.  It’s just taken me that long to get around to this series.  (There’s been a lot of other stuff to talk about in the meantime, such as SolidWorks World 2009, something called a 3D mouse, and rants about this or that.) The Part 1 article in this series discussed how to make, place and size Empty Views.  Part 2 now discusses how to use them once they are created.

Use Empty Views as quick Zoom to selection locations

OK, let’s say that one empty view each represents the title block, revision block and drawing notes.  How does one quickly move about the drawing to view these areas?  There are several methods available in SolidWorks.  The following method is likely less common, but is perhaps quicker can more common methods.

First, assign a shortcut to Zoom to selection function.  Zoom to selection is found under View pulldown>Modify>Zoom to selection.

Zoom to selection location

To add the shortcut (for much quicker access to this function), goto Tools pulldown>Customize…>Keyboard tab> and then search for “zoom to selection”.  From there, simply add a keystroke as the shortcut for Zoom to selection and choose OK to save.

Now here is how to use this shortcut with Empty Views.  With the drawing open and with no views selected, look over in the FeatureManager.  Select any one of the Empty Views (or any view for that matter).

FeatureManager display of views

As this point, simply hit your shortcut keystroke for Zoom to selection.  The viewport will immediately zoom to the area identified by the Empty View.

Zoom to selection of empty view

Choose another view from the FeatureManager and hit your shortcut for Zoom to section again.  Each time, the viewport will immediately zoom to the area defined by the selected view.

Using Empty Views for PDF bookmarking

As an added bonus, any views created on the drawing (including Empty Views) will become bookmarks if you save that drawing as a PDF.  This adds greatly to the navigability of PDF files for everyone who uses them.  Within PDF Reader, the bookmarks will appear to the left (similar to the FeatureManager in SolidWorks).  Simply LMB click on the desired view, and PDF Reader will jump to that location.

There are some pitfalls with saving a drawing as PDF, so if your company is experiencing those, then it is not recommended that drawings be saved as PDF.  In those cases, print to PDF works better.  Unfortunately, bookmarks are not created when printing a drawing to PDF.

Conclusion

The one thing that frustrates me about SolidWorks Empty Views is that SolidWorks Corp reduced their functionality (as discussed in Part 2).  However, with a simple hack, they can be used as drawing bookmarks, to contain drawing notes,  and to add functionality to PDF files.  Additionally, they are always useful for containing sketches, as noted in Part 1 of this series.

Using Empty Views (Part 2: Creation)

In this article I’m going to cover how to create an Empty View, and the ugly hack for making it a desired size.  In Part 2, I will cover how to use Empty Views for quick zooming and bookmarks in PDFs.

Creating Empty Views

Creating Empty Views is easy.  With a drawing open, goto Insert pulldown>Drawing View>Empty.

Add empty view to drawing

SolidWorks will then ask for a location on the drawing for the Empty View. Simply LMB click at the desired location.  In the example below, I’ve placed the Empty View in what might seem to be an very unusual location (covering the Revision Block table).  I’ll cover why in Part 2 of this article.

Pick location on drawing

Ugly Hack

To get the Empty View to stretch across the full length of the Revision Block table, we’ll need to employ an ugly hack.  Within the new Empty View, draw a line that starts from the corner of the border. Terminate the other end at the vertex of the table at other end.  The endpoints of this line will not attach to these two vertices, but will drop on top of them when the line is created.

Pick location on drawing

The result is an Empty View sized as required. The way to hide the line in this hack is to place it directly over another line (in this case, the Drawing Border).  (A RMB click on the line and choosing the Hide function will not work.  The view will resize back to its default shape.)

Pick location on drawing

Now RMB click on the view and choose the Lock View option.  This will keep the view in place (preventing it from accidentally shifting around).

Making the Empty View useful

To make this new Empty View useful, rename it in the FeatureManager.Renaming the Empty ViewRenamed Empty View

This will allow for easier identification when it comes time to use this (and any other Empty Views).  Part 2 will explain more about this and the reason for these additional steps.