Category Archives: SW2007

SolidWorks World 2014 Proceedings are available now!

I hope every enjoyed their time at SolidWorks World 2014  at the San Diego Convention Center, San Diego, CA. It was great to be a part of the event and meet lot of people.

This year also there were lot of interesting presentations and hands on sessions were conducted by various professionals including SolidWorks employees, SolidWorks Users and SolidWorks VARs. And like everyone, I was also waiting for them to get these presentation and videos upload for access to everyone.

So the wait is over now and the SolidWorks World 2014 proceedings site is now available.

Visit http://www.solidworks.com/sww/proceedings/ to acceess the proceedings information.

Be sure to take full advantage of this year’s proceedings site. Watch breakout session videos, download breakout session PowerPoints and check out photos from this year’s event. Also, view the 2014 highlights video and videos from general session each day.

Hope to see you at SolidWorks World 2015 in San Diego, CA!

P.S. The copyrights of the video content on this web site are owned by DS SolidWorks. Unless otherwise specified, DS SolidWorks only grants you the right to view the video content on this website

Alternate Position or Configuration in SolidWorks

Do you ever need to show open/closed positions or parts movements in drawing views. Let’s take an example of Box Cover Assembly to explore two different ways of presenting the required views.

Alternate Position View Method:

1. Start a drawing and place the assembly view as required.

2. Right click on view and select Drawing View > Alternate Position View or go to View layout and click on Alternate Position View. You’ll be prompted to select a view if not selected.

3. Alternate Position View will generate a new configuration in the assembly. So give the desired configuration name and click OK.

4. The mode will change to assembly from drawing.

5. Set the part(s) in desired position and click OK. (P.S. There has to some parts in the assembly that are not completely fixed else you won’t be able to drag/move them to new position).

6.  The drawing will get updated with Alternate Position View shown in dotted in the same view.

Configuration Method:

1. Open up the assembly and switch to configuration mode.

2. Add a new configuration named Opened (or you may give  a different name too).

3. Set the part(s) in desired position (by editing mates) so that both configuration have different part(s) position(s).

4. Save assembly and start a new drawing.

5. Place the desired view.

6. Right click on drawing view and select properties.

7. In the Drawing View Properties dialog box, under Configuration information,  select Use named configuration and select the Opened configuration from the list. Click OK.

8. The view configuration will change to Opened configuration and part(s) position(s) will get updated as per configuration.

9. If required you may show two different views showing open and closed positions.

Exploding a Multi-body part -2

Continued to my earlier post on exploding a multi body part, here is another example.  I have used a Weldment part for his example.

Example 2: Exploding a Weldment Part.

1. Click here to download the SW2011 part files used for this example.

2. Unzip and open up Weldment Part-2011 file.

3. Set the “3DSketch1″ to show. Right click or click on “3DSketch1″ and select show.

4. Also make sure sketches are set to show under View menu.

5. Go to Insert > Features and select Move/Copy Bodies

6. Select the two bodies as shown in the pic under bodies to move/copy.

7. Expand Translate (as we want to move out the body) and give 15mm as Delta Z value.

8. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in Z direction.

9. Restart Move/Copy Bodies command using step 5 or right click any where on the graphics area and select Recent Commands > Move/Copy Bodies. You’ll have to restart the command for further steps.

10. Select the side body as shown. Select the “3DSketch1″ line for direction and give -15 as the distance value.

11. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

12. Select the two bodies as shown in the pic. Give -15mm as Delta X value.

13. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in X direction.

14. Select the side body as shown. Select the “3DSketch1″ line for direction and give -15 as the distance value.

15. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

16. Select the two bodies as shown in the pic. Give -15mm as Delta Z value.

17. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in Z direction.

18. Select the side body as shown. Select the “3DSketch1″ line for direction and give 15 as the distance value.

19. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

20. Select the two bodies as shown in the pic. Give 15mm as Delta X value.

21. Click OK to close the close the command and apply the changes. The bodies have moved out by 15 mm in X direction.

22. Select the side body as shown. Select the “3DSketch1″ line for direction and give 15 as the distance value.

23. Click OK to close the close the command and apply the changes. The body has moved out by 15 mm.

24. You may hide the “3DSketch1″ if required. Right click or click on “3DSketch1″ and select hide.

25. You may add two configurations one showing collapsed bodies where as other one showing exploded bodies.

26. Download the completed SW2011 part file here.

Exploding a Multi-body part -1

Many of us have been dealing with multi body parts and sometimes we need to show an exploded view similar to what we do in assembly to give a presentable picture of the parts or to show more details. Creating an exploded view in assembly is quite easy using the tool available. But are there any ways to replicate same in a multi body part.

Let’s explore the ways to do it:

Assembly Method: The easiest method is to convert the multi body part to assembly using this quick method : Assembly from Part – No mates required and then explode them using the exploded view tool.

Part Method:This particular method takes the advantage of move/copy bodies. Let’s discuss this method with some examples.

Example 1: Exploding a Multi Body Part.

1. Click here to download the SW2011 part file used for this example.

2. Unzip and open up Multi Body Part-2011 file.

3. Go to Insert > Features and select Move/Copy Bodies.

4. Select the “Side Plug” body (the blue colored) under bodies to move/copy.

5. Expand Translate (as we want to move out the body) and give40mm as Delta Z value. You may give direction or value for the move/copy if required for your parts.

6. Click OK to close the close the command and apply the changes. The “Side Plug” body has moved out by 40 mm in Z direction.

7. Restart Move/Copy Bodies command using step 3 or right click any where on the graphics area and select Recent Commands > Move/Copy Bodies.

8. Select the two “Round Plugs”.

9. Expand Translate and give 25mm as Delta Z value.

10. Click OK to close the close the command and apply the changes. The “Round Plugs” have moved out by 25 mm in Y direction.

11. You may add two configurations one showing collapsed bodies where as other showing exploded bodies.

12. Download the completed SW2011 part file here.

To be contd… Check Part 2 here

UP-Down through the Feature Tree

Many of us sometimes needs to see that how a model has been built up in SolidWorks. The most commonly used method is to move scroll bar up in the feature manager tree and then move it step by step down. Using mouse for this process can be tedious sometimes.

STOP here. If you also use this method and looking for something easier, then continue reading and learn anew method.

  1. Start SolidWorks and go to Tools > Options or click on Options.
  2. Click on Feature Manager under System Options.
  3. Select (check) “Arrow Key navigation“.
  4. Click OK to apply and close the system options.
  5. Roll back the feature manager tree.
  6. Click on the scroll bar.
  7. Using Up-Down arrow keys, you can now move the scroll bar up or down as required.

Other funtions you can achieve with arrow keys

To …                                                              Press:

scroll up                                                       up arrow

scroll down                                                  down arrow

collapse the design tree                               left arrow with pointer at top of design tree

expand the design tree                                right arrow with pointer at top of design tree

collapse an item                                           left arrow with pointer at item

expand an item                                            right arrow with pointer at item

drag the rollback bar up                              up arrow with rollback bar selected

drag the rollback bar down                         down arrow with rollback bar selected

Creating a Form Tool for Sheet Metal Parts

There are two different methods to create a form tool. I’ll be creating a very simple Emboss tool with an open face (which means that particular face will be removed from the sheet metal part when this form tool is applied).

Old School Method (can be used with older version also):

1. Start a new sketch on Top Plane.
2. Start a rectangle of any size.
3. Add an equal side relation between any two perpendicular sides (optional).
4. Give dimension to any of the side (optional). I have given 2 in as the linear dimension. This will fully define the sketch.
5. Now click on Extrude Boss/Base feature on the feature tool bar or Insert > Boss/Base > Extrude.
6. Extrude in any direction to any thickness. I have used .1 in as extrude thickness and click OK  to exit the command.
7. Start another sketch on the top face.
8. Draw a circle any where on the face.
9. Give a dimension as per requirement of tool size. I have used .5 in as diameter of the circle.
10. If required you can define the position of the circle to make the sketch fully defined though this is not required.

11. Extrude to the height you want for the tool using Extrude Boss/Base feature. I have extruded to .2 in height.
12. Now click on Fillet/Round feature on the feature tool bar or Insert > Features > Fillet/Round.
13. Add a fillet of .1 in on the selected edge (ref. picture).
14. Now start a new sketch or use the same sketch used for creating the rectangular base and do a cut extrude. I have used the same sketch. Sometimes it is good/easy to create a new sketch and use it.

15. Select sketch1 from the feature manger tree and click on Extrude Cut feature or Insert > Cut > Extrude.
16. Using any option i.e. Blind, Up to surface or Vertex, cut away the rectangular base.
17. The final shape will look like as shown in the picture.
18. Start a new sketch on the highlighted face (ref. picture).
19. Click on Convert Entities feature or Tools > Sketch Tools > Convert Entities.
20. A fully defined sketch will get created on the selected face.
21. Click OK to exit the sketch command. Now rename the sketch. To do this, select the Sketch in the feature manager tree and press F2 on the keyboard (shortcut for rename) or Select the sketch, pause and then again select to start the rename option.
22. Rename the sketch to Orientation sketch.
23. Now add colors to the faces to define the form tool. Right click (RMB) on the face, click on appearances and then click on Face to start the appearance mode.

24. Add color in this manner. Stopping face: Cyan color, Faces to Remove: Red Color and rest all faces Yellow color.
25. Now it is the time to save the form tool in the proper location.

26. Click on File > Save or Save as (in case you’re editing an older form tool).
27. Browse to the location where you want to save the tool (you can save either in the forming tool folder under design library or create a new folder in case you want to share the form tool over a network). Give a proper file name (I have used Dia .5 X .2) and select Form tool under File type. I have created a new folder under forming tool folder in design library with the name “My tools” to save/store the new form tools.
28. Save the file and you’re done.

New Method (Available from SW2007 onwards):

1. Repeat steps 1 -17 as discussed above. You might not require creating a base in some shapes. You need a base only if you need a fillet at the bottom.
2. After you have create the shape required, go to Insert > Sheet Metal > Forming Tool or click on Forming Tool feature on the sheet metal toolbar.
3. Select the required face as Stopping face.
4. Select the required face(s) under Faces to remove.
5. Click OK to exit the command.

6. The required colors will be added to faces as per the selection and a sketch with the name Orientation sketch will be added on the stopping face.
7. Save the files as described in steps 26- 28

We’ll see how to use the form tool, mapping the file location so that it can be shared over a network in another post.

Diagonal cut on a Cuboid-2

This is in continuation with Part 1, here is another method to cut a diagonal on a cuboid

Using Loft:

1. Open the existing file or create a new file and model the cuboid.
2. Start 3D sketch.

3. Select Line command.

4. Select any one vertex of the cuboid.

5. Start the line and while in line sketching mode, select the second vertex.

6. Continuing with the sketch, select the third vertex.

7. And finally select the first vertex you started sketching with.

8. The final sketch will look like in the picture (might differ if you have a different sized cuboid).

9. Now click on point command.

10. Create a point on another vertex (leaving the three vertices used above).

11. Exit sketch mode and switch to loft cut (select from toolbar or Insert > Cut > Loft cut).

12. Select the 3D line sketch as first profile and point as second profile. If you have the “show preview” selected, you can see the preview.

13. Select point as second profile. If you have the “show preview” selected, you can see the preview.

14. Click OK and end result will be the diagonal cut.

Customize Custom Property List

Do you ever wanted to edit the Custom Property List you see under Property name in File Summary Information. You might have to remove or add any additional property or even reorder the list. Here are the few easy steps to achieve that.

1. Close any open SolidWorks session. Though this will not make a difference but might be better sometimes if the list is in use.

2. Browse to this path \\SolidWorks\lang\english (can be different in your machine) or search for Properties.txt file in the director where SolidWorks has been installed.

3. Create a backup copy of this file, just to make sure you can use it again if required. You may rename the backup copy as Properties_Old.

4. Now open the Properties.txt file with any text editor (e.g. Notepad)

5. Add any additional property that you want to see in the list, remove any unwanted property or edit the order of the list in the required manner. I have added two properties Test1 and Test 2.

6. Save the file (either by File > Save or Ctrl + S).

7. Start SolidWorks, open or start a new file and check the list under File Summary Information.

8. You can also keep/copy the edited Properties.txt file over shared folder or network so that every SolidWorks user has access to same file.

9. If you’re copying the file over shared folder or network, make sure you add the path for the file under Tools > Options > File Locations > Custom Properties List.To add the file location, click on Add and browse to the file location.

10. Also the same file is used for name under Custom Property Attributes in Property Tab Builder.

Using Sketch for dimensioning in Drawing

There might be situations when you need to use a sketch to show some dimension in a drawing.  You simply turn on the sketch and create the required dimensions.

Now next thing will be to hide the sketch as you don’t want to show it up. So you simply right click on the sketch in the feature manager and set the sketch to hide.

Oops, to your surprise, the dimension which you have created have also puffed off (or better to say they hide too). Now if you turn the sketch on (or show) then only you can see the dimensions which you don’t want. So here is simple trick to get what you need.

  1. Set the sketch to show and create the required dimensions.
  2. Right click on the sketch in the feature manager and set the sketch to hide.
  3. Now is the real thing. Right click on the sketch in the feature manager and select show dimensions.

Hurray, you have the dimensions back to live (which you have created earlier) with your sketch hidden.

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 advice 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.