Category Archives: Tables

SOLIDWORKS: Controlling Scale Features in Configurations

We all use Scale feature in the model to quickly scale up or down a model. The idea is to quickly change the geometry of the model for various purpose. For e.g. in a plastic mold, components are usually scaled up to take care of shrinkage. The scale value depends on the plastic material. It does not scale dimensions, sketches, or reference geometry but only the model geometry (body). One can scale a solid or surface body about its centroid, the model origin, or a coordinate system depending on the requirements.

Applying a Scale:

1. Open the model you want to apply scale to.

2. Go to Insert > Feature > Scale OR use Scale icon from the toolbar.

3. Select from the drop down for “scale about”

4. Fill in the required value and click OK.

5. Scale feature is added to the model.

You can scale selected bodies in case of a multi body part.

You can also scale with different values of X, Y and Z directions by deselecting uniform scaling and adding required values for X, Y and Z directions.

Now if you have various configurations, you can easily control the scale factor value for them using two simple methods.

Method 1: Scale Property Manager (might not work for older versions than 2014)

1. Open the Model having the configurations

2. Go to Insert > Feature > Scale OR use Scale icon from the toolbar.

3. Select from the drop down for “scale about”

4. Choose uniform scale or uncheck it.

5. Key in the desired scale value.

6. If you have more than one configuration in the model, then you would see another box for the configuration selection. Select the desired option and configuration accordingly.

7. Click OK and Scale feature is added to the model.

Method 2: Design Table

1. Open the Model having the configurations.

2. Insert a design table (Insert > Tables > Design Table) OR edit the existing design table

3. If you already have a scale feature then it should get added to the design table. If not then add the column headers for controlling the scale feature.

4. In case you want to keep the uniform scale, add column header as $X_AXIS@Scale Feature Name and desired value for each config.

5. In case you want different values for X, Y and Z directions, then add three column headers as $X_AXIS@Scale Feature Name, $Y_AXIS@Scale Feature Name, $Z_AXIS@Scale Feature Name and desired value for each config.

6. Exist the design table and your scale feature in now controlled via design table.

Fixing eDrawings SOLIDWORKS Document Manager Issue

eDrawings is free software that lets you view and print eDrawings (eDRW, ePRT, eASM), native SOLIDWORKS documents (sldprt, sldasm, slddrw) , DXF, and DWG format files.

Download eDrawings

The eDrawings Viewer is intended primarily for people who do not use CAD software and thus do not need to publish eDrawings files themselves. This means people can use this program even if they don’t have SOLIDWORKS. But some people might see following error while running eDrawings on their machine.

eDrawings SOLIDWORKS Document Manager Error Message

If you get similar error then it is possibly related to either SOLIDWORKS Document Manager older version or SOLIDWORKS Document Manager is not installed on your machine. As per SOLIDWORKS Knowledge base* (SPR #: 627955), this issue is related to mainly x64 machines. To fix simply install the latest version of SOLIDWORKS Document Manager. You can download latest version of SOLIDWORKS Document Manager here.

Please report back to your VAR if you’re still getting the error message even after installing/updating SOLIDWORKS Document Manager.

*Active subscription required to access SOLIDWORKS Knowledge base

Making your Drawing Tables Jump in SolidWorks

This particular topic comes often in various SolidWorks forums that “Can the Tables be moved to another sheets in a Drawing“. The answer is simply Yes and there are various ways to move them to different sheet.

Let’s check the various tables used in SolidWorks first:

In this post, I will be trying to discuss various ways using which one can move these tables to different sheet in a drawing.  You can use any of the methods below to move the table onto other sheet. I have used BOM table to explain these methods and some of the methods explained below might not work on all types of tables.

Cut and paste Method

1. Click on the table you want to move (in the drawing area).

2. Press Ctrl + X (cut) on the keyboard or Edit > Cut.

3. Activate the sheet you want to move the table onto by right clicking on it in the manager tree and select Activate or click on it in the sheet tab.

4. Press Ctrl + V (paste) on the keyboard or Edit > Paste.

5. Your table is now on new sheet, you can set its position as required.

Drag Table Method-1

1. Select the table you want to move from manager tree by clicking on it.

2. With the table selected, keep the left mouse button pressed and drag the table below the sheet name on which you want to move the table onto.  Pay attention to change in pointer when you do that.

3. Your table is now on new sheet, you can set its position as required.

Drag Table Method-2

1. Click on the table you want to move (in the drawing area).

2. With the table selected, take your pointer to the cross (refer picture).

3. Keep the left mouse button pressed and drag the table on the sheet name (in the sheet tab area) on which you want to move the table onto.  Pay attention to change in pointer when you do that.

4. Your table is now on new sheet, you can set its position as required.

Multi Configuration in Assy BOM

Do you know you can show multiple configuration in single BOM. Check the steps to know how to do it in case you need it.

The assembly I have used here has two configurations, named Full and Cut Out. The difference is the number of clamp part plus cutout in one of the configuration.

  1. Insert the drawing view as required.
  2. Insert BOM table by right clicking on the View, selecting Tables > BOM OR select the inserted view and then go to Insert > Tables > BOM
  3. If you don’t have a view selected, you’ll be prompted with a message to select a view.
  4. You can select the view by clicking on it.
  5. Now BOM property manager will appear. Under BOM Type select “Top Level only” and under Configurations, select all the configurations or the required one. I have selected all in the list i.e Full and Cut Out.
  6. After setting up the options, click on OK.
  7. Place you BOM as required OR if you have a fixed anchor, you can set the BOM to attach to anchor under table position in BOM property manager. Check the quantity of desired parts. In this case it was the Clamp part whose quantity is correct as required.