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.

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.

Motion along Path

As the name suggest, the post talk about creating a quick animation of part(s) along a path. The path can be open or close. And to illustrate the method, I have used very simple parts (a box and a path).

Preparing for the animation:

1. To start, create a rectangular box of any size.



2. For the path, you can create a new part with the path (basically a sketch) or start a new assembly, start a new part and create the path or simply create the path sketch at assembly level ( I have used the path created at assembly level by creating new part).



3. Insert the box into the assembly containing the path (sketch). Make sure you have set the box to float in case if it is fixed by default.
4. Position your box by applying the suitable mates. I have used one coincident mate to freeze some of the degrees of motion/freedom.



5. Now define a path mate. Start Mate manager and under Advanced Mates, select Path Mate.



6. For Component Vertex, select the part vertex to attach to the path (you can select any vertex as per the condition or your part placement).



7. For Path Selection, click on selection manger. (If you have converted the path to a single spline then you just select the sketch for defining path without using the selection manager option).



8. Switch to Select closed loop option in the selection manager.



9. Now select the sketch defined for path (the whole sketch will get highlighted).



10. Click OK to define the path.



11. Under Path Constraint, select Distance along Path and set the value to 0. Keep rest of the settings unchanged.



12. You may select/uncheck Flip dimension to change the direction.
13. Finally click OK to define the mate and exit mate manager.



Tip: Measure the full length of the path (using measure tool to define the distance value). You may also convert the path into single spline (using fit spline option). This facilitates easy selection without using the selection manager in defining path.

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

Creating the animation:

1. Save your assembly (any location and name as desired) and switch to motion manger/study. Set the view orientation as required.



2. Drag the timeline any time value.



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



4. Key the desired value and click OK to finish distance modifications.
5. Now hit calculate and then finally you can play/save you animation.

Tip: You can hide the path if desired.

Here is the link to video: Path Mate

Enjoy playing with motion along different paths.

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.