Adding Sketch length to Part properties

This is a very simple example on representing sketch length (individual or total length of sketch) in the part properties.

1. Start a new sketch or edit exiting one.

2. Dimension the sketch as required. Make sure you add the chord/arc length to any radius entities (click here to see how to create an arc length dimension) instead of radius value (if required you can set the chord/arc length as driven dimension.

3. Within the sketch mode, start an equation by either right clicking on the equation folder or Tools > Equations

4. You can use any name for this equation (I have used Total length as I’ll creating a total sketch length).

5. Set the equation equal to sum of all the 3 dimensions (can be more or less as per the sketch). You can also set equations for individual dimension.

5a. Add = sign after the equation name

5b. Click on the dimension you want to add. You can select the dimension in any order.

5c. The dimension name will appear in the equation editor.

5d. Add + after the dimension name.

5e. Select the second dimension you want to add, add the + sign and finally select the last dimension. If you more dimensions to add, keep on repeating till you select the last dimension (don’t add any sign after the last dimension name).

5f. Make sure you select the chord/arc length dimension and not radius dimension.

6. Finally click OK on the equation editor (to exit the editor).

7. You can see the finally evaluated vale in the equation manager. The value will be different in your case.

8. Click OK on the equation manger to exit it. And you may also exit the sketch edit mode.

9. Go to file properties.

10. Under custom/configuration tab, add the required name under Property name (I have used Total Length here also as the property name)

11. Select text under type from the drop down list.

12. Finally select the equation (as created in step 3 above) under value/text expression from the drop down list.

13. The final value will appear under evaluated value.

14. Click OK to exit the property manager/summary information.

15. Now you can link your notes to this property.

Do you use a different method? If yes, how about sharing the same.

Thanks

Adding / Removing Jogs

Just a quick presentation on how to Add or Remove a Jog

What is JOG? There can be several answers for this question but if we talk in engineering, the answer might be adding bends to an entity. The entity can be a line (2d sketch or 3d sketch), a note leader or a linear dimension extension line.

Click on the pictures to read in detail on How to Add OR Remove Jogs on specific entities.

Adding Jog to a linear dimension extension line

1. Add your dimensions as required.
2. Right click (RMB) on the dimension extension line and go to Display Option > Jog.

3. You’ll notice two points created on the dimension extension line where you did the right click. If you can’t see that just click once on the dimension extension line.

4. Now select drag that bottom point (or point closer to dimension text, refer pic) and set the jog.

5. To remove the jog, select any of the points (as seen above) and hit delete on the keyboard.

Adding Jog to a Note Leader

1. Add your note as required or use any existing note (to which you want to add the jog).

2. Right click (RMB) on the note leader and select Add Jog.

3. You’ll notice another point created on the leader where you did the right click. If you can’t see that just click once on the leader.

4. Now select drag that point and set the jog.

5. To remove the jog, select the point (as seen above) and hit delete on the keyboard.

Adding / Removing Leaders

You use leader with notes or other annotations is SolidWorks. Depending on the need you may add a single leader or may be multiple.

And while adding multiple leaders, you may add an extra leader which is not required and you want to omit that. This post talks about adding as well as removing leader from a note or annotation.

Adding a Leader

1. Click any where on the Leader.

2. Select the point on the arrow head.

3. With Ctrl and left mouse button pressed (will be right hand button in case you use a left hand mouse), drag the arrow to any side.

4. Place the arrow pointing to an entity, edge, face or leave open.

Deleting a Leader

5. Now in continuation of above, assume you added an extra leader and what to get rid of that.

6. Click any where on the Leader.

7. Now click on the point of arrow or extra leader which you want to remove.

8. Press delete on the keyboard. Bingo, the extra leader has gone.

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.

Deleting a Row from General Table

This question came up on the SolidWorks Forums today and after answering it I thought of sharing it up.

You have inserted a General table in the SolidWorks drawing and accidentally added one extra Row. Now you want to get rid of that line. As usual you’ll right click on the specific Row you want to remove from the table and clicked on the Delete.

But to your surprise, you can only see the option to delete the entire table and no Row. You may feel bit frustrated with that.

Now here comes the trick to delete the Row from the General Table.

1. Click on Table and you’ll see some thing like in the picture below.

2. Click these small arrows to show the Table Header. (Check, the pointer has changed).

3. Your table should like this.

4. Click on the table again.

5. Select/ highlight the Row (by clicking on the number. See the color change). Now right click on the row number, go to Delete and select Row.

6. Hurray, the unwanted Row has gone. If you want to hide the table header, click on the table again. Now click on those small arrows (look at step 2) again and your header will hide.

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.

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.