Hole color

Mark,

Edit: Attached a VBA macro and re-wrote the explanation.

See attached for a VBA macro that will change newly added hole wizard features to red. You will see in the commenting where I show you how to use Case statements to modify the color depending on the type of hole wizard hole. There's a tremendous number of hole types, so please look in the swWzdHoleTypes_e enumeration to find exactly what you want.

Explanation: To get the feature colors to change automatically upon feature creation then you need to use event notifications. As Artem points out below, it is not enough to use AddItemNotify, since this fires before the rebuild, but also OnIdleNotify, which fires once SolidWorks is "idle" again. The itemName argument in AddItemNotify is used to get the name of the newly added feature. Finally, IFeature::SetMaterialPropertyValues2 is used to actually change the color. Note that the first three arguments of the array in correspond to RGB (on a scale of 0-1) so you need only change them to change the color.

The disadvantage of event-triggered macros is that you already need the macro to be running. Consequently, to ensure that its always on, you can change your SolidWorks shortcut to run the macro when SolidWorks is launched. I show you how to do that in this blog post: 4 Ways to Run A Macro Without the Run Button. To see more examples of notification macros, check out our Macro Library.

Alternatively, you could just write a macro that you run manually, which searches the feature tree for hole wizard features, determines their hole wizard type, and colors them accordingly.

Keith

Video Tutorials for the SolidWorks API

I'm afraid the AddItemNotify is not enough in this case. At this moment feature is not completely created (this is not post notification). Changing the feature in this state may be risky. For example on my end it changes the whole body because separated entities are not yet generated for feature.

It is better to use some post notification.

Furthermore I would not suggest to use VBA macros because you need to have some User Form or something like that to keep them 'alive' after it ends. The best choice is to use add-in however the VSTA macro should also work because you can toggle the SolidWorks settings to not close the debugger when macro ends (added to macro directly).

You also need to keep track of the documents change and attach to active document every time.

I have implemented this in C# VSTA macro, please find this in the attachment.

Try to run it and to create a "Through all counterbore" in hole wizard and it will be colored to red. You may change the list of colors and features in the block in 'main' procedure:

            //TODO: add your types here

            m_Palette.Add((int)swWzdHoleTypes_e.swCounterBoreThru, Color.Red);

            m_Palette.Add((int)swWzdHoleTypes_e.swTapered, Color.Green);

            m_Palette.Add((int)swWzdHoleTypes_e.swCounterDrilled, Color.Blue);

You may also change the features itself's slightly modifying the macro. but I would finally suggest to switch to add-in and forget about running the macro at all because you can run the add-in on startup automatically,

Hope it helps.

__________________________

Regards,

Artem Taturevych

Application Engineer at Intercad

http://intercad.com.au/

Tel: +61 2 9454 4444