As the name suggests, this topic covers the SolidWorks Installation FAQs. If you have questions like; what should I do to my system prior to a new installation? Or how do I uninstall SolidWorks from my computer? Or why is it recommended to turn off anti-virus scanning when installing SolidWorks? Then this post is a must read to clear all your doubts. If still you have anything other than covered here, please write back or comment.

Click here for SolidWorks Installation FAQs

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.

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.

When one thinks of slot, generally the obround shape comes into mind. I have seen various posts where a user has asked about making a slot or obround cut. There can be several ways to create a slot and one may adopt the method which he/she finds easy and quick to use. In this chapter let’s discuss about various ways of making a slot.

1. Line –Arc Method: Start a new sketch and start a vertical or horizontal line as desired. You can choose the line command from the sketch toolbar or press L (a keyboard shortcut for line command, for more keyboard shortcuts and customization, go to Tools > Customize> Keyboard). Now without exiting the sketch press A (a shortcut for Arc), a tangent arc will get started from the end point of your line. Create a semicircle with the arc command and the moment you finish the arc, the tool will get switch back to line command. Finally press A again to switch back to arc command and finish your slot. Though the tangent relations between the arcs and line should come automatically but sometimes one may not use line arc method correctly and there can be different shape. In that case one can add the tangent relation manually by selecting the two entities (line and arc) and then select the tangent relation in the property manager.

2. Circle-Line Method: Draw two circles (can be of equal diameters if required) and create a construction line (vertical or horizontal) or add a relation (vertical or horizontal) between their centres. The reason of putting a line or adding relation is to constrain the two circles. Now start line and draw two lines from the quadrants of one circle to the quadrants of another circle. Using trim tool, remove the unwanted area of the two circles and your slot is ready.

3.  Circle-Rectangle Method: Using the above method create two circles and constrain them. Now instead of using line command, pick rectangle and keep the starting point on one quadrant point and finish the rectangle by dragging the other point to the opposite quadrant of second circle. Trim away the unwanted area and add the tangent relations if required.

4. Rectangle-Arc Method: Create a rectangle and exit the rectangle command by pressing ESC or jump to next command i.e. tangent arc. Create two semi circles on either sides of the rectangle. Trim or delete the unwanted area and add the tangent relations if required.

5. Offset/End Cap Method: I really like this trick/method. It is the easiest and quickest method to create a slot. Create a line (vertical or horizontal) and exit the line command. Select the line and click on offset command or vice versa. In the offset property manager, give the distance value, select the option “Bi-directional” and then select “Cap Ends”. Under make end caps, select arc. If you have the preview on, you can see the preview for the slot. You may select the option “Make base as construction” if you haven’t created a construction line or if you want to covert the line into a construction line. Click OK and your slot is ready.

6. Slot Tool/Sketch Method: This is a new innovation in the slot making in SolidWorks with lot of options while making the slot sketch. The sketch tool contains slot geometry too. To use the tool, go to Tools > Sketch Entities.

Apart from creating vertical or horizontal slots, one can create an angled slot by using angle dimension.

Also there can be different ways to dimension a slot. One can adopt the method his/her as per the company standards or what he/she feels is best for them to use.

Perfect, you can now play with different methods of slot creation. Do add if you know any other method I missed out.

]]> http://gupta9665.wordpress.com/2009/06/12/different-ways-to-make-a-slot/feed/ 4 Boxer sl1 sl22 sl3 sl4 sl5 sl6 sl7 sl8 http://gupta9665.wordpress.com/2009/06/11/how-to-animate-simple-spur-gear-in-solidworks/ http://gupta9665.wordpress.com/2009/06/11/how-to-animate-simple-spur-gear-in-solidworks/#comments Thu, 11 Jun 2009 04:38:48 +0000 Deepak Gupta http://gupta9665.wordpress.com/?p=312 ]]>

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

Sorry for keeping this one longer. There was some other work going on which kept me away from putting this one up but I’m happy to have this one now..

To start you will the spring file you created in the last chapter i.e. HOW TO ANIMATE A SPRING -1.

1. Open the spring part file.
2. Click on the Record button on the macro tool bar. If you haven’t have the macro toolbar one, you can go to Tools > Macros > Record to start recording. To show the macro toolbar go to View > Toolbar > Macro.

3. Double click on the spring body to show the dimensions and then click on the length, 100 mm in this case if you used the same old spring part file.

4. In the pop up window change the value to anything > I have changed it to 110 mm.

5. Click on Rebuild in the same dimension box or from the toolbar.

6. Finally click Stop on the macro toolbar or Tools > Macros > Stop.

7. Give a name your macro and hit save. I have used Spring Animate.

8. Now click on Edit button on macro toolbar or Tools > Macros > Edit

9. Browse to the macro you saved in the step 7 and open it.

10. VB editor will get open up and your screen will look like this.

11. Remove the extra line and make your window look like this.

12. Copy these 3 highlighted lines and paste them.

13. The editor window will look like this. Change the system value to .1. The system takes all in puts in meter. So if you want any other value convert it to meter and put here. .1 denotes .1 m i.e. 100mm

14. Add these 4 lines as shown and save you macro. You can keep any value for “i”. In this case I have used 10 which means the macro will run for 10 times. You can give any value or can create an input box where user can put the number of steps he needs. I will put up a macro or tutorial on how to do that.

15. Close the VB editor and back to SolidWorks window. Click on Play button on macro toolbar or Tools > Macros > Play

16. Browse to the macro you edited and saved in step 14.

17. Now sit back and enjoy the animation.

Apart from using macro, I have been trying to use Phil Sluder’s trick (SW Tips/Tricks – July Issue Adding Logic to Equations) but getting some error. I have requested Phil to check the same. As soon as he fixes as where I’m going wrong, we can have animation of spring using equations too. I’m also going to put another one using a combination of equations and Animator.

Link for the macro used in this tutorial: Spring Animate.swp

Different ways to mate with a SLOT-2…

Different ways to mate a square/rectangular part with a cylindrical part…

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.

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

1) Start a new part. Right click on the Material and select Edit material from the pop up menu.

2) Right click any where on the left side and select New Library.

3) Save you database a name and at a specified location or Solidworks default Location. I have used My_mat09 as my database/library name.

4) The new material database/library will get added in the list.

5) To add a material category, RMB on the new library and select new category.

6) Give a name to the new material category. For e.g. Steel, plastic, etc. I have used My_Mat.

7) To add you new/customized material, RMB on the new category and select new material.

8 ) Give a name to you new material. I have used XYZ_1. Start editing / filling in the properties by double clicking in the value cell. You can get these properties from various website over internet or material handbooks.

9) Set the appearance and cross hatch for the material.

10) After editing / filling in all the details, click on apply and then close to exit the material editor.

11) Great you just have made you own material database. You can see you new material in the list.