SOLIDWORKS drawing

Objective

We want to create notes using properties such as description, material and mass in the 3D model, and transfer this information to the SOLIDWORKS drawing.

The purpose of these notes is simple: they are updated when the 3D model properties are modified, so that they automatically fill your title block.

Take a 3D model with volume:

Create custom properties

Several solutions are available:

• Use SmartProperties from the myCADtools suite

• Use SOLIDWORKS property forms

• Create properties manually

In this tutorial, we're going to create the properties manually. To do this, go to File / Properties or click on the "Custom Properties" button:

Note: if you're using configurations, some of them will have to be created in the "configuration properties" tab.

We will create 3 properties:

• Property name => Description_Type => Text _Value/Text expression => Test (this property must be filled in manually)

• Property name

  => Material (available in the drop-down menu) _Type=>Text _Value/Expression => SW_Material property (property linked to your choice of material, so automatically filled in)

• Property name

  => Mass (available in drop-down menu) _Type => Text_Value/Text Expression => SW_Mass property (property linked to the volume/material so automatically filled in)

Let's move on to the layout

This model has an incomplete title block, as the 3 properties created in the 3D model have not been integrated.

First of all, create a view of any kind to create a link between the 3D and 2D files. We obtain a partial filling of the title block information:

Go to the "Plan background" tab and click on "Edit plan background". We're now going to add the 3 properties we've created to the 3D model.

Go to the "annotation" tab: and click on "note": click to select where you want to create it, then go to the Property Manager.

This is where we'll create a property linked to a 3D model issue. Click on the property button

The menu will be displayed:

To access the properties of our 3D model, it will be necessary to select model found here 2 (3D model) instead ofcurrent document (drawing). Once done, go to the property name drop-down menu 3 and select the desired property (here, the description property).

Once you've confirmed the previous dialog box, you can use the formatting toolbar to set the text to the desired size and font:

In the title block, we obtain the following result:

Note: If you leave the mouse over the note, you can see the syntax used by SOLIDWORKS($PRPSHEET: "Description") if you wish to create properties without going to the "property-related" menu.

All you have to do is repeat the operation for the following properties:

You can now quit editing the plan background.

Although our example here was created by inserting properties in the title block, it is perfectly possible to perform the same operation on plan views, as in the following example:

The advantage is, of course, that the duplicated plan references the new part, so you don't have to recreate it. There are several ways of duplicating a part and its drawing, while ensuring the link between the new drawing and the new part.

Using the SmartProperties tool in the myCADtools suite

Thanks to the SmartProperties tool in the myCADtools suite, you can easily create a new model and its associated drawing from an existing model. In fact, by modifying property values, SmartProperties will calculate a new name and suggest that the user generate a new 3D document by managing the duplication of its associated drawing(s).

The reference link of the new drawing will then be automatically modified to the new 3D model.

Copy/paste method

The simplest method is to copy and paste in Windows Explorer. To illustrate this method, let's take the example of a part A.SLDPRT and its associated drawing A.SLDDRW :

• First, Copy/Paste the files A.SLDPRT and A.SLDDRW into a new folder, then rename the 2 copied files to B.SLDPRT and B.SLDDRW.

• Then simply open the B.SLDDRW drawing with SOLIDWORKS , telling it that it now refers to B.SLDPRT instead of A.SLDPRT. To do this, in SOLIDWORKS, click on "File/Open", select the B.SLDDRW drawing and instead of clicking on "Open", click on the "References" button:

Next, the window that opens allows you to edit the location of referenced files. In our case, the file referenced by B.SLDDRW that appears is A.SLDPRT. Double-click on A.SLDPRT, and use the explorer that appears to select your new B.SLDPRT reference, then confirm by clicking on "open":

The result of the replacement is then displayed in the editing window.

Click OK to confirm, then "open" in the "file/open" window. You must then accept any update requests.

Finally, plan B.SLDDRW opens and now points to part B.SLDPRT. You can check this by clicking on "File/Check references". All that remains is to save the plan.

In SOLIDWORKS assemblies, it is possible to plan layout cuts directly at the design stage. Let's take a look at how to create a SOLIDWORKS drawing cut and a cutaway view from a 3D assembly.

Section view in 3D

First of all, to plan the drawing cut, simply use the SOLIDWORKS "cutaway view" tool by clicking on in the upper view bar. Then make the same settings as for a 3D cut.

However, before confirming, you can select the parts you do not wish to cut in the drawing. As shown in the image below, simply activate the "Cut by component" dialog box and select the part(s) you do not wish to cut in the drawing (excluding fastener parts, which will be generated automatically).

On the other hand, if you wish to select components not to be cut in the drawing at a later date, this is possible.

For example, in the assembly below, we have chosen not to cut the axis indicated by the red arrow.

Finally, to save your section view, simply click on the "Save" button at the bottom of the Property Manager.

SOLIDWORKS drawing options

After clicking on the "Save" button, the following window appears.

To retrieve this section from your drawing, you need to check the "Drawing annotation view" option. Then click on "Save" again to bring up the second dialog box.

At this stage, it is still possible to select components not to be cut during the drawing cut. You will also find the "standard" drawing options, such as automatic hatching and the exclusion of fasteners.

Finally, click on "OK" to finish.

Show section view in drawing

To retrieve the cut defined in the 3D model, use the view palette, then drag the view used to create the cut, followed by the cut itself. The cut will automatically be displayed in "cut" mode, with the components you had selected in "uncut" mode.

On the other hand, you can of course modify the components to be excluded from the cut in the traditional way. To do this, right-click in the cut view "property". Then select the components to be excluded in the "cut extent" tab.