Linking Dimensions (values) – 2

Continued from part one, this post discuses the second method i.e. “Shared/Link Values method”

Shared/Link Values:

When dimensions are linked in this way, any member of the group can be used as a driving dimension. Changing any one of the linked values changes all others to which it is linked.

The variable name you specify becomes the name of the linked dimensions.

How to use Share/Link values to link two dimensions:

1. Start a new part and start a sketch on any of the plane. Draw a rectangle with any size.
2. Start dimensioning and give dimension of any one of the side but don’t click OK.
3. Click on arrow next to dimension and from the list select “Link Value”
4. Next you’ll see “Shared Values” window.
5. Give a variable name in the box (I have used W as variable name) and click OK to come out of the shared values window.
6. Click OK and come out of this window. Now you can see a link symbol in front of the dimension indicating that this is a linked dimension.
7. Now dimension the other side, click on the arrow in the dimension value modify box and select Link Value.
8. In the “Shared Values” window, click on the arrow and you can see W in the list.
9. If we want to keep both the values same, select the W from list else write a new variable (in case you want to link this dimension to a different one). As I’m linking both of them to each other, I have selected W. Notice the change of value.
10. Click OK and come out. You’ll see the similar link symbol as it is there in front of other dimension.
11. Change any of the dimension value and see the effect on the second one.

This was really a very example of using/creating linking dimension value. And similarly you can create many linked dimensions with different variable name and values.

Linking Dimensions (values)–1

As the post name suggested, here we will discuss on ways you can link two or more dimensions. The basic idea is make dimensions depend on each other and helps in quick updation of the dimension value.

The two ways via which dimensions can be linked are:

1. Using Equations
2. Shared/Link Values

Both the methods can be used in parts as well as assemblies.

Using Equations:

When dimensions are linked in this way, one member of the group is a driving dimension and second or others are driven dimension(s). Changing the value of driving dimension will change all others driven dimensions as per the equation has been set.

I have used a very basic sketch (rectangle) to explain the methods of using equations and link values.

How to use equations to link two dimensions:

1. Start a new part and start a sketch on any of the plane. Draw a rectangle with any size.
2. Start dimensioning and give dimension of any one of the side.
3. Dimension the other side but don’t click on OK.
4. Click on arrow next to dimension and from the list select “Add equation.”
5. You’ll see a add equation window pop up with the current dimension there (“D2@Sketch1” in this case) with = sign.
6. Now select the dimension already created in step 2 above and you’ll see that is added after = sign in the add equation window (“D1@Sketch1” in this case).
7. Now the equation is “D2@Sketch1” = “D1@Sketch1” which means the value of “D2@Sketch1” will be same as of “D1@Sketch1” (1.000” in this case)
8. Now say I want “D2@Sketch1” to be half of “D1@Sketch1”. Simply add /2 at the end of the equation. Now the equation will look like “D2@Sketch1″ = “D1@Sketch1″/2.



9. Click OK to come out of equation editor and you can see the equation listed in the equation window.
10. Click OK to come out of equation window. You can notice the equation symbol in front of the dimension indicating that this is a driven dimension.
11. Change the driving dimension value and see the change in the driven dimension value.

This was really a very example of using/creating equations. You can try lot of other settings, values, etc. in equations. And similarly you can create many equations.

Animating a Can Crusher

This has been already discussed on SWGeeks.com so I thought of putting it in form of an article so that other can refer this.

Can Crusher: A can crusher is a device used for crushing aluminum soda cans for easier storage in recycling bins. While most recyclers don’t require you to crush cans, if you do recycle a lot, your normal bin may fill up quickly. The can crusher gives you extra space by flattening either single or multiple cans.

The first can crusher was of course the human foot. People often stomped on cans to flatten them down either for recycling or for greater space in the garbage can. This could sometimes hurt if the foot did not come down properly on the can, so entrepreneurs eagerly sought a variety of alternatives that could be used with the hand.

(Source http://www.wisegeek.com/what-is-a-can-crusher.htm)

There are many types of can crusher viz. mechanical, hydraulic. The one discussed over here is one of mechanical type which has two gears (having rotary and linear motion, driven by a hand wheel). The can is crushed by forcing it against solid plates which moves along with the gears.

As this post is all about animation, I’ll not go into details of how to model the parts. This post focus mainly on rotary and linear movements/motions of the two gears. Some of parts have not been shown / modeled for clarity purpose. I’ll be using the files shared by Lavanya on SWGeeks.com

The parts used for this animation are Side Cover (not shown in the pic below), Cover/Body, Rack, Gears and Hand Wheel.

1. Start a new assembly and properly mate the following parts viz. Cover/Body, Side Cover and Rack.

2. Insert the two gears (with shaft and without shaft) in the assembly and position them appropriately.

3. Create a gear mate between both the gears. Make sure the ratio is 1:1. You have to place the gears so that there is no interference.

4. Insert the hand wheel and mate it with the Gear (with shaft) so that both can rotate/move w.r.t each other (for further steps, I have the hand wheel hidden for better clarity).

5. Now is the real trick. Don’t use Rack and Pinion mate in this animation as that will not work. Gabi already pointed it out on here blog. Instead of Rack and Pinion mate, I have used two distance mates. Create two distance mates between gear axis and side face/cover. The distance value for both the mates should be same.

6. Add an angle mate between the side face and corresponding parallel plane of either of the gears. I have used plane of gear (with shaft).

7. Now you have completed most of thing and it’s time to do some animation.

8. Switch to animation/motion study mode and set the view orientation.

9. Drag the time line to some distance (w.r.t. time). I have set to 5 seconds.

10. Change the value for all the three mates, two distance mates (changed values should be same) and third that angle mate (you can change the value to 360°).

11. Click on Calculate and then finally you can enjoy with the animation.

Wow, the gear are rotating along with hand wheel as well as moving forward. Here is the link to video.

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.

Different ways to Mate with a SLOT -1

Now we have finished and learned the techniques of making a SLOT, the second question comes up in the mind is “How to Mate with a SLOT”. Again there can be several ways to achieve this and one may adopt the method which he/she finds easy and quick to use. In this chapter let’s discuss about various simple ways of mating with a SLOT.

To use these methods you need a simple plate with a Slot of any size, a cylindrical, rectangular or square part with diameter/width equal to or less than slot width. In this chapter I’m going to use the cylindrical part (pin). I will be covering another discussion on same topic with a square part too.

Start you assembly with the plate inserted as the base part and fixed. You can also use mating techniques to position your plate. Now insert you pin which you want to mate with the slot.

Method 1: With your assembly opened and both the part inserted, select the back face of the plate and bottom face of the pin. Add a coincident mate between them. You can select front and top faces too. This is to set the initial position. Now show on the temporary axis (View > Temporary axis) to display the temporary axis of the pin. Select the side face of the plate and the temporary axis of the pin and give a distance mate. Repeat this with the bottom face. Your pin is now in to the required position.

Method 2: Using the same technique as described in method 1, use the planes instead of the temporary axis of pin to give distance mates with the side and bottom faces of the plate. Your planes may vary from the one shown in the picture.

The difference in the above two methods is that in Method 1 the part is not fully define and its free to revolve on its axis whereas in Method 2, the part gets fully defined.

Method 3: This is a combination of above 2 methods. Add a distance mate using the side face of the plate with the corresponding plane of the pin. Now show up the temporary axis if they are not on. Select either of the temporary axes of the slot and corresponding plane of the pin. Add a coincident mate.

Method 4: If your slot width and diameter of the pin and equal then you can use this method. Add a tangent mate between the side face of the slot and the cylindrical face of the second part. Then add a distance mate with the bottom/side face depending upon the location of your slot with the corresponding plane/temporary axis of the pin.

or

Method 5: In this method, RMB on the edge of the plate and select “Midpoint”. Then select the corresponding plane of the pin and add a coincident mate. Then add a distance mate with the bottom/side face depending upon the location of your slot with the corresponding plane of the pin.

Method 6: This is tricky method and I prefer to use this method most of the time. Open the plate and edit the slot sketch. Add these two construction lines to your slot sketch. Now in assembly, select to show the slot sketch. Use the planes of the pin and mate them with the corresponding construction line

These are few of the methods which I use for mating with a slot. I would be interesting to hear if you more methods or any other method that you use for mating with the slot.

How to animate simple Spur Gear in SolidWorks

In this post I will discuss about a simple animation of Spur Gears. I have used SW2009 for the tutorial but lower version can be used to perform this activity. You can use any cylindrical part for the animation. I have used spur gear to make the animation more realistic.

1. Start SolidWorks and go to Tools > Add-Ins. Make sure Toolbox/Toolbox browser is checked. If not then check them to add.

2. Click on the right side on Design Library and Select Toolbox. Next select Ansi Metric > Power Transmission > Gears. In side pane, you will see gears, racks, etc. RMB on Spur gear and select “Create Part”.

3. Set any properties of Spur Gear as desired. Click OK and then save your part.

4. Now click on “Make assembly from part/assembly” icon or File > Make assembly from part/assembly to start a new assembly.

5. Drop the gear anywhere in the assembly. It will get fixed by default.

6. RMB on the part in the feature manager and select Float from the pop up window. This will remove the fix constraint from the part and make it free to move/rotate.

7. Now show the temporary axis by View > Temporary Axis. You can also use part axis if there is any to proceed.

8. After you have made the temporary axis on, the view will be like this.

9. Select the center axis as shown of the gear.

10. Select the appropriate plane (Front plane is this case) and click on Mate if it doesn’t pop up (as in pic) from the assembly toolbar.

11. Set a coincident mate between the selected plane (Front) and axis.

12. Select the same axis and another plane (Top plane in this case) and add another coincident mate.

13. Select the front face or back face of the gear and the left over plane (Right plane in this case) and set another coincident mate.

14. Now the part is constrained in such a way that it can rotate free around its axis. Check it by dragging the gear. You will see the rotary movement only.

15. Select the gear in the workspace or feature manager and drag it while keeping the Ctrl button pressed. This will create a copy of the gear.

16. Mate the front faces of both the gear by adding a coincident mate between them.

17. Select the center axis of second/copied gear and appropriate plane (Top plane in this case) and add a coincident mate.

18. Select the center axis of second/copied gear again and either a plane or center axis of first gear (I have selected Front plane) and add distance mate. I have given 10mm. You can set the position by flipping the direction.

19. Now the second/copied gear is also free to rotate around its axis. Check this one also by dragging.

20. Set both the gear in an appropriate position as shown.

21. Click on Mate; go to mechanical mate and select gear mate.

22. Select the center axis or any other faces. I have selected the bore faces. Set the ratio to 1:1 as they are same gear and finally click OK. You can try with different sizes of gears.

Your gears are ready to animate. Try to drag any of the gear and see the other gear rotate. You can also add a rotary motor to animate the gears.

Click here: Gear Animation Files.zip

How to make a 3D PDF out of SolidWorks

There is possibility of creating a PDF output where a user can do not only rotate, pan and zoom but there are many other functions one can see in the created PDF. In simple word you can get a 3D PDF out of SolidWorks. This option is available from SW2007 onwards.

1. Open any part or assembly file for which you want to create the 3D PDF.

2. Go to File > Save As

3. In type file type, select PDF

4. Select “ Save as 3D PDF”

5. Finally save your file.

Perfect you have a created a 3D PDF

1. Open the 3D PDF file.

2. RMB or right click anywhere in the graphics area to see what other functionality are there.

Great Start playing now. Do explore more functions. I have tested this PDF in Adobe reader version 7.0 and above. All the functions showed above are from Adobe Reader 9.0 and may not be working in lower versions but rotate, pan and zoom work fine.

Click here to download sample 3D PDF file.

HOW TO ANIMATE A SPRING -1

Quite many time people have been asking me as how I have done the spring animation or can we animate spring in SolidWorks. The answer is yes and here is the trick. I have used SW07 to show “How to Animate a Spring”.

1) Start a new part (can be either mm or inch).

2) RMB on the top plane or any plane and choose “Insert Sketch” from the pop up window. You can also select plane and click “Insert Sketch” from the tool bar or menu.

3) RMB anywhere in the graphic area and select circle from the list. You can also select circle from the sketch tool bar or menu.

4) After you have drawn the circle RMB anywhere in the graphic area and select Smart dimension.

5) Dimension your circle. It is always a good practice to use fully defined sketches. You can give any value, I have used 80mm.

6) Exit sketch. Now with your sketch selected or you can select it later, go to Insert > Curve and select Helix/Spiral. You can select the same from feature toolbar.

7) Set your parameter in the Helix/Spiral Property Manger. I have used Defined by: Height and Pitch. Parameter: Constant Pitch. Height: 50 mm. Pitch: 10mm and Start Angle: 0 deg.

8 ) Click OK and exit the Helix/Spiral command. Now RMB on right plane and select Insert sketch. You can create a new plane if you set any other value to the start angel. Select Plane from the tool bar or from the menu list and then select the Helix or vice versa. In the plane menu select the option “Normal to Curve” if it is not selected by default. Now start a new sketch on the new plane.

9) Draw a circle and dimension it. I have set the value to 8mm.

10) Select the center point of the circle and CTRL select the helix i.e. press CTRL for selecting the Helix. In the property manger select the Pierce relation to fully define the sketch. The black color indicates a fully defined sketch.

11) Select Swept Bose/Base command from the toolbar or got to Insert > Bose/Base > Sweep.

12) In the property manager, select the circle as the profile and helix as the path and click OK. Your spring is ready.

13) Now double click on the spring to see the helix dimensions.

14) Double click on the pitch dimension (10 mm in this case) to edit it. In the pop up window click on the arrow next to dimension and select “Add Equation” from the list.

15) You will see the equation manger with pitch dimension (D4@Helix/Spiral1) on the left side followed by = sign. Now click one on the Spring Height (50mm in this case i.e. D3@Helix/Spiral1).

16) After clicking on the Height the equation will look like “D4@Helix/Spiral1” = “D3@Helix/Spiral1”. Put a / after “D3@Helix/Spiral1” and either manually give the number of revolution or select the number of revolution (5 in the case i.e. “D5@Helix/Spiral1”).

17) Try changing the height and do a rebuild. You will see the pitch changing.

Perfect, you have completed the first/main part for animating the spring.

Link for the part: Spring.sldprt

HOW TO CREATE ISO SECTION VIEW-2

Continuing with the old ISO section trick, SolidWorks has added a good option to create an isometric Section View.

1) Create the drawing placing/creating any view except Isometric or similar view.

2) Create section view and place the view.

3) RMB on the sectioned view and select the Isometric Section option from the menu.

4) You are done with the Isometric Section View.

HOW TO CREATE ISO SECTION VIEW-1

Many times people have been asking about how they can create an Isometric Section view. When I started working on Solidworks, I used the configurations trick to accomplish this. Now a day I call that as an old trick. I have used one simple revolved part for this exercise. This trick can be applied to assemblies as well. Here goes the old ISO section trick.

1) Create one configuration of the part/assembly of which you want to show the ISO Section.

2) Give any name as per the convenience. I have used Iso Section.

3) Now create a rectangle on the face, either half or one quarter. I have used one quarter.

4) Create a full cut extrude.

5) Save you part and switch to Default configuration.

6) Create the drawing placing/creating an Isometric view.

7) Now RMB on the view and select properties.

8 ) Change the configuration from the pop up window.

9) Your view will look similar to shown below.

You can also skip steps 5-9 by placing the Iso Section configuration on the first view itself. I just wanted to show another option also.

10) Go to Insert, Annotations and select Area/Hatch fill or select from the toolbar.

11) Select the two faces in the Isometric view. Set the type, scale, angle etc. of the hatch and click OK.

12) You are done with the Isometric Section View.