Graphics Systems SolidNotes

Getting WMF out of SolidWorks

Often times people want to get nice, vector-scalable artwork out of SolidWorks for use in technical publications. An easy way to do this is to make a blank drawing sheet with the view(s) you want, and then save it as an Adobe Illustrator file. For Tech Pubs departments that use higher-end publishing tools, that works just fine.

However, what if you're a smaller shop and you don't have Adobe or Quark products? What if you use good ol' Microsoft Word? In the past, you could just bring DXF files into Word, but that functionality actually went away in Word 2003 -- I was as suprised as anyone when I found that out! So, then what? Word can't take in an AI file. You could print the SolidWorks drawing to a Postscript printer file, and then manually doctor it up so that it looks like an EPS, but that's kinda dark arts type stuff (and the resulting file wouldn't have a TIFF preview). Are you condemmed to using raster images in your Word documents?

Not if you have a little $38 program called docPrint. It's from an innovative little company called VeryPDF. They have all kinds of useful tools for dealing with document and image format conversion. I was able to get vector-scalable line art from SolidWorks drawings, and also get very high-quality, scalable art from SHADED views, right from the 3D model, using this software to make Windows Metafiles (.wmf and the newer "enhanced" .emf). You can even try it for free to make sure it works for what you want to do. Check out www.verypdf.com and look for the docPrint product.

Leveraging 3D Annotations

We help many SolidWorks users become more proficient and efficient with the tools they use everyday. Simply having such a potent MCAD software at their disposal is a gigantic step towards productivity gains.  And yet, it surprises me when I ask users if they take advantage of leveraging Annotations from their 3D model in to their 2D drawings.  Few do. (But if you are one who does, shout out; we'd like to hear from you)  In the end, we're talking about saving you time in the creation of your 2D drawings.

The first and easiest tool/technique is to insert Annotations such as Datum symbols and notes at the 3D model level. (Insert, Annotations from the pull-down menus) To view these annotations, right-mouse click the Annotations folder in the model's feature tree and choose "Display Annotations."  The particular Annotation type can be set within the Details of the same context menu.   Then, to bring these Annotations into drawing views on the print, use Insert, Model Items from the drawing's pulldown menu. Click on the thumbnailed images below to view the screenshots.

A second technique is to use 3D Annotations along with a special drawing view type called Annotation Views.  This method likewise speeds up the time it takes to document our 3D work. Additionally it is useful for quickly conveying manufacturing design intent per the ASME 14.41-2003 standard.  3D Annotation Views are organizer according to the model's orthographics projections (Front view, Top view, etc) and can be created manually or automatically.  As a warning, however, 3D Annotation Views are not dynamically linked back to the model from whenst they came. To re-create the drawing view and show updated annotations, the view will have to be deleted and re-inserted.

How do I create an Annotation View?- From within the model, you can create an Annotation either dynamically (while you are inserting Annotations) or by marking an orientation as a Annotation View and selecting items after the fact.  Again, from a right-mouse click on the Annotations folder, check off "Display Annotations" and "Enable Annotation View Visibility." Also from that menu, you can create a new Annotation View. (Insert Annotation View)

The desired Annotations can be selected after choosing the orientation (or face) you wish to control. Follow the blue arrows as they direct you through the wizard.

The last piece of the puzzle is to create the views in your 2D drawing.  From within the drawing, insert a new drawing view from the model.

Select the radio button marked "Annotation View" and whatever views exist will be highlighted; also, note the little letter "A" next to the icon.  See the thumbnail below.

Creating efficiency with SolidWorks is easy and there are many unique techniques such as this to help you along. 

Min/Max Your Dimensions

SolidWorks has three different attachment points when dimensioning a distance to and arc or circle. The arc conditions are described below.

Center: The default when an arc is selected. Dimension attached to the center point of the arc.

Minimum Distance: Attachment point is to the closest point on the arc on the same die of the center as the other end of the dimension. Linear dimension does not cross arc centerpoint.

 

Maximum Distance: Attachment point is to the farthest point on the arc on the opposite side as the other end of the dimension. Linear dimension crosses arc centerpoint.

Selecting an arc as part of a linear dimension causes the dimension to default to the center arc condition. However, if the Shift key is held down as he arc is selected for a linear dimension, the arc condition will be minimum or maximum, whichever is closest to the side being selected.

Further, the arc conditions) of a dimension can be changed after the dimensions is created. Right-click on the dimension, select Properties, and  change the arc condition by selecting the new option near the bottom of the dialog box.

Note that there can be two arc conditions to control if the linear dimension is between two arcs.

Why can't I have Configuration Specific part numbers in my BOM?

Actually you can, and there are two different ways of doing it...

The first is to have the configuration name be the part number.  To do this you must go into each and every part and subassembly and change the Bill of Materials Options (inside Configuration Properties, as show) for each configuration in the model.  This sounds like a big task but That's what it's gonna take.  You are goin to have to change it from saying Document Name (SW Default) to Configuration Name, and then name each configuration what you want it to be.

 

 

 

 

The second, and preferred by me, way is to use a configuration specific custom property.  The trick to using a custom property is that the Bill of Materials Options (inside Configuration Properties, as show) must be set to User Specified Name and $PRP:"PartNumber" (where PartNumber is the name of the configuration specific custom property being used).  Again this initial change must be made to each configuration in every single part and sub assembly in your assembly. 

Here are several reasons(In no particular order) as to why I prefer this method:

 

 

• Confugurations can be named as you please
• Custom properties are easier to edit than configuration names
• Changing a custom property will not affect the ability for an Assembly to find the correct configuration
• Part number can be controlled in the same place as all the other properties in a model
• All the other items in the BOM are custom properties (or should be, and I mean it)

 

Here's another tip when doing this... An easy way to tell if all the configurations in a particular model are properly set, is to simply look at the configuration tab and to the right of the configuration's name it should say [ $PRP:"PartNumber" ] as shown.

 

And now for the best part... to all of you who bothered to read this whole article I am including a macro that will add a configuration specific custom property to each configuration and rename the Bill of Materials Options to User Specified Name with the value set to show the property name specified. Click Here to Download  The use of this macro is at your own risk.  Graphics Systems Corporation is in no way responsible for any damages that occur as a result of using this macro.  The macro is provided as is and will not be supported in any way.

All of the knowledge necessary to write this macro can be achieved through the SolidWorks API class offered at Graphics Systems.  Please see our class listings for the next available class.

Them's the Breaks!

I often get the question, “Why don’t my dimension lines break when I turn on the Break Lines option in my dimension properties?”

There is a little-known switch on the Dimensions page of the Document Properties that can have a major affect on the Break Lines option:

When active, Break around dimension arrows only causes the system to do just that: only dimension lines that cross arrows get broken. Clear the switch and you’ll get the behavior you’re looking for.

Gimmie my auto view projection in 2007!

There are a number of great enhancements in SolidWorks 2007, but one of them is personally not my cup of tea. In drawings, one of the new 2007 enhancements is the View Palette. This is the new palette available from the Task Pane that shows you all of the defined views of a particular model. While I like being able to snatch a view from the View Palette once I'm working on a drawing, I don't like how it works when I'm first creating a drawing from a model. I prefer to have the Insert Model View command pop up and let me place projected views the old way. If you want to restore that behavior to your own 2007 installation, it's easy to do through a SolidWorks system option. Tools > Options > System Options, and in the Drawings category you will find "Show view palette." Turn that off and the View Palette won't jump out in front of you when you make a new drawing.