Tag Archives: Assembly

SolidWorks Cutaway Animation

SolidWorks Cutaway Animation

Hi All, sorry for being too late in posting this one. So before putting any further delay here are the steps by steps on doing “SolidWorks Cutaway Animation”. Please note that you should have SolidWorks Professional OR Premium installed in order to access the animation/motion manager.

If you’re reading this for first time do check this completed animation

Download the files you would need for this animation here. The files are in SW2013 version.

1. Open the assembly SolidWorks Cutaway Animation.

2. Set the three default assembly planes to show (optional, but make it easier in selection).

3. Insert a part named Cutting Plate and drop it anywhere in assembly.

4. Select the top face of Cutting Plate and add a distance mate for 140 mm between assembly top plane and top face of the Cutting Plate.

5. Rotate the view and go on the back side.

6. Select the face shown and add a coincident mate with Right plane (important).

7. Select the face shown and add a coincident mate with Front plane (important).

8. You may now set the three assembly plane to hidden state (in case you’ve set them to show).

9. Select the top face of Cutting Plate and start a new sketch (important).

10. Now click on the convert entities to get the sketch we need for this animation (I’ve set the Cutting Plate to hidden state for clarity).

11. With the sketch active, go to Insert > Assembly Features > Cut > Extrude.

12. Set End condition as thru all. Under Feature Scope uncheck “Auto Select” and then select the components you want to cut thru.

13. Click OK to exit the sketch/cut feature mode. Test the set up by changing the distance mate from 140mm to 5mm. You should see the cut feature in the assembly. Keep the distance as 5mm only (optional).

14. In case you don’t see the cut, then please change the cut-extrude direction.

15. Once you set it up, then switch to motion study tab. Please note that you should have the MotionManager selected under View menu.

16. In the motion study tab, drag the slider to any time (in this I’ve set it to 6 sec).

17. Expand the mates folder.

18. Double click on the distance mate we have set between the top plane and cutting plane. Set the value back to 140mm. Click OK to set the distance.

19. Now you should see the blue lines in the motion manager which represent change in the vale.

20. Finally click on calculate button and enjoy the animation.

You can add motors to the shaft to get more realistic animation. I’ve used PhotoView360 to process this animation shown below.

SolidWorks 2013 Sneak Peek: Any Component as Envelope

With almost 2 days to go for the release of SolidWorks 2013, here is one more interesting feature to share with you. SolidWorks 2013 gives you the ability to make envelopes from subassemblies. Workflow improvements include designating components as envelopes as you insert them into assemblies, and changing components to or from envelopes at any time. New options let you adjust envelope visibility and load envelopes as lightweight or read-only.

A quick video on the new feature

Need more on what’s new in SolidWorks 2013, visit new SolidWorks 2013 website to see all the major updates when it launches on September 10, 2012.

SolidWorks 2013 Sneak Peek: Exclude Components During Interference Detection

With only few days left for the big event i.e. release of SolidWorks 2013, here is another cool feature of SolidWorks 2013. You can exclude selected components in Interference Detection  in SolidWorks 2013, . You can filter components with matching cosmetic threads from Interference Detection results and place them in a separate folder. You can exclude interferences involving hidden components, as well as exclude selected components from Interference Detection results. Optionally, you can specify to remember components to exclude from session to session.

This video shows how this applies to cosmetic threads.

Need more on what’s new in SolidWorks 2013, visit new SolidWorks 2013 website to see all the major updates when it launches on September 10, 2012.

SolidWorks 2013 Sneak Peek: Mates in Mirrored Subassemblies

Here’s yet another new feature for 2013. When you create an opposite-hand version while mirroring a subassembly, all the standard mates in the subassembly are mirrored as well. Previously, standard mates within the subassembly that mated to the default planes or origin of the subassembly were not created..

A quick video on the new feature

Need more on what’s new in SolidWorks 2013, visit new SolidWorks 2013 website to see all the major updates when it launches on September 10, 2012.

SolidWorks 2013 Sneak Peek: Insert Multiple Components in Assemblies

Here’s another new cool feature for 2013. In the Insert Components PropertyManager, you can select multiple components at a time and then insert each one in succession without returning to the Property Manager. Also, if you double-click the assembly origin, all the selected components are inserted at once, each with respect to the origin.

A quick video on the new feature

Need more on what’s new in SolidWorks 2013, visit new SolidWorks 2013 website to see all the major updates when it launches on September 10, 2012.

Different Mate Values for Different Configurations

Do you ever need to set up different mates vales (Distance and Angle mates) for different configurations in the Assembly.

You can download the files used from here to do this exercise/tutorial.

1. Open the Assembly the switch to configuration manager.

2. Add the configuration as required. I already have two configurations in the assembly: Closed and Open.

3. Activate the configuration named Open.

4. Expand the mates folder.

5. Double click on Angle1 mate (so that the dimension displays up in the graphics area).

6. Double click on the dimension.

7. Set the value to 120 and set the option “This Configuration

8. Click OK to set the value and exit the dimension edit box.

9. Rebuild if required.

10 Switch to configuration manager and check both the configurations.

Similarly you can set different values for distance mate too in your assemblies.

Flexi Tube -1 (motion thorough a tube)

Just another fun with the SolidWorks animation. This one talks more on in-context modeling approach and how to use that for animation. Though more focus will be on creating the animation but yes there is small though most important role of in-context modeling.

Preparing for the animation:

1. To start, create a spherical ball of any dia and the save the part as Ball ( I have taken the dia as 3in).

2. Start a new assembly and save it with any desired name and preferred location.

3. Insert a new part via Insert > Component > New part*.

4. Select front plane as the base plane for new part. You may choose a different plane too.

5. Create a sketch on as shown in the pic (you may choose different values for the dimensions).

6. Using revolve feature, create a cylinder and finally exit the part edit mode. You may save the part internally or externally as desired.

7. Now insert the ball part (created in step 1) into the assembly. Place it any where in the assembly and make sure it is floating i.e. not fixed.

8. Add two coincident mates (between front planes of ball and assembly and similarly between top planes of ball and assembly).

9. Add a 1.6in value distance mate between right planes of ball and assembly.

10. Now switch to part edit mode and edit the long tube/pipe (created through steps 3-6). You can right click on the part in graphics or in the feature manager and select edit part.

11. Start a new sketch on the front plane of the pipe.

12. Expand the feature tree for ball part and select the sketch used to create the ball.

13. Click on convert entities. This will copy the sketch used for ball onto the front plane of the pipe

14. Using horizontal line as centre line, create a revolved feature.

15. Hide ball part for easy selection and further feature addition/editing. Right click on the ball part and select hide components.

16. Add a fillet of 0.25in as shown.

17. Add a shell feature with 0.1in as wall thickness, shell outward and select both the ends of the tube under faces to remove.

18. Create another sketch on the front plane of the pipe (as shown) and do a revolve cut.

19. Exit part edit mode. And finally save the assembly.

You have finished with doing the required steps prior to animation.

* If you are using SW2007, then you’ll have to save the part externally but in higher versions, you can save the part internally in the assembly. Check SolidWorks help for more details on it.

Creating the animation:

1. Switch to motion manger/study. Set the view orientation as required.

2. Drag the timebar to any time value (I have set it to 10 seconds).

3. Now double click on the distance mate mate. This will highlight the distance value and dimension modify window will pop up.

4. Key the desired value (I have used 13.5in) and click OK to finish distance modifications.

5. Now hit calculate and then finally you can play/save your animation. Check the video under My Videos section.

Enjoy playing motion with different shapes/sizes.