Category Archives: SW2010

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

Animating Geneva Mechanism in SolidWorks

I’have been seeing lot of people talking on Geneva Mechanism over various forums and even I have been wondering myself on animating a Geneva Mechanism in SolidWorks. In the past I had used many different tricks to achieve it like gear mates or using surfaces etc.

Here is an animated view of what I have done few days back. I have been modelling some simple file to put up for this post but I recently came across SolidWorks Geneva-Device files on GrabCAD by Bobby Dyer. I would like to thank him for allowing me to use his files to create this tutorial.

Based on the requirements Geneva Mechanism can be external or Internal:

     

You can download the files used for this tutorial here: SolidWorks Geneva-Device files.  The important ingredient are Contact and Motion Study Properties

1. Open the “Geneva Device” assembly from the downloaded files.

2. Switch to Motion study and set the model orientation as required.

3. Change the Motion study type to “Basic Animation“.

4. Click on “Contact“.

5. Now in the Contact property manager click on the pin to keep it visible as we need to use it twice.

6. Now under components selection box, select “Index Wheel” and “Advance stop” parts.

7. You can select them from graphic area OR from feature manager tree OR motion study tree.

8. Click OK to apply the contact.

9. With Contact property manager visible, select “Index Wheel” and “Indexer” parts and click OK to apply the contact. You can now close the Contact property manager.

10. Click on “Motor“.

11. Set the motor type to “Rotary motor“. Select the cylindrical face or circular edge of “Index Wheel” or “Indexer” parts to define the direction of ( I have selected the cylindrical face of the Indexer). Set the motion function to “Constant Speed” and RPM to 30.

12. Click OK and apply the motor.

13. Now click on “Motion Study Properties“.

14. In the Motion Study Properties property manager under basic motion, set the frames per second to 30 (the larger number the more smoother motion) and set the Geometry Accuracy and 3D Contact Resolution settings to high side (move the sliders to right). This will make collision simulation more accurate and smoother motion, but requires more time to compute.

15. Click OK to set the properties.

16. Finally click on “Calculate“.

17. And now is the show time. Hit play to enjoy the show.

You can change and experiments with the settings to get a better animation. Click on save if you want to export the animation as AVI or series of pictures. You can change other settings in the save window.

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

SolidWorks Functionality Survey

 

SolidWorks team is looking to better understand what aspects of SolidWorks you are using and roughly how often you are using them. The information will help them as a guide for future product developments.  The survey will not take much time to complete.

Please take the survey here

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.

Creating Animations with SolidWorks step-by-step

Animation had always been an interesting thing for me and I keep on doing experiment with animation in SolidWorks. SolidWorks has recently come up with its new version of “Creating Animations with SolidWorks step-by-step”. And when I was asked for reviewing the book I was full of joy as this will be my first chance to learn more about the animation from a step by step guide.

The book contains 35 easy-to-understand tutorials and practice exercises, each building upon the previous lesson. The best thing is that everything has been explained via step by step, enhancing your skills on SolidWorks animation as you progress from simple to more complex animations. There are case studies and practices files included at the end of each chapter to make your grip more stronger on animation and revise what you have learned through out the chapter.  Total 536 pages book which also include DVD-ROM containing files (SolidWorks 2010 version) for tutorials and practice exercises. The book costing $89.95 can be order via SolidWorks online store.

The quick overview is that it’s a good book every SW animation beginner or who wants to enhance his/her skill with animation, should have this book as there is lot of stuff to try and learn. I’ll be posting more about the book as I progress with the chapters blogs. You can also learn more about the book on Gabi Jack and Rob Rodriguez blogs

Chapter 1: Explains what is Animation, why it is required and how to create it. And what different types of Animations can be created with SolidWorks Animator.

Chapter 2: Explains easy steps on creating simple animation and get you started with animation. Also discusses on saving the animation.

Chapter 3: Explains editing the timeline and key points.

Chapter 4: Explains creating/editing and tweaking the view orientations. Also explains use of perspective view.