For those of you who use the Enterprise PDM add-in for SolidWorks, you know that the little preview on the Enterprise Task Pane is small and hard to see. So while looking around in the Knowledge Base the other day, I ran across how to remove the preview and leave more room for the other information you want to see in that area.

All you need to do is make a quick change to the Windows Registry.

IMPORTANT: Only make changes to the Windows Registry at your own risk. Create a backup before making any changes.

1. Close SolidWorks
2. Click on the Windows Start icon
3. Type regedit in the Search box and select it from the list.
4. Go to HKEY_CURRENT_USER\Software\SolidWorks\Applications\PDMWorks Enterprise\ConisioCAD\SolidWorks
5. Right click on SolidWorks > New > DWORD
6. Name the new entry BitmapPreview
7. Right click and select Modify
8. Set the value to 0 (zero)
9. Reopen a file from the vault in SolidWorks and check the Task Pane.

You can resize to expand the horizontal column and you will have more room to view the properties.

Keep checking – I plan on adding more quick tips for EPDM.

When creating a sheet metal part in SolidWorks, one of the key features is the capability to “Flatten” the model into a sheet so it can be manufactured. This allows the manufacturing entity to have a flat pattern drawing derived from the created part.

There may come a time when the product needs to be produced from round bar stock. Being that this component is not sheet metal, it cannot be flattened. This would prompt the modeler to create two separate parts, one for the bent shape and one for the unbent shape.

What I am going to show you is a technique I developed that will allow you to one create a part that contains two configurations; one bend, one unbent. The goal is to create the two configurations of a horse shoe shape product made from bar stock.

1. Create a section of round bar stock. This is basically a round extrusion that has a .25in diameter and 10in length. You can use Extrusion, Sweep or any other method to create the base shape.
   
2. Locate and activate the Flex command. You can do this by using the Command Search function in Solidworks.  Simply type “Flex” in the search bar, this will populate results as you type. Then click the glasses to see the location of the Flextool.
     
3. Now the Flex Manageris open on the left side of the screen, for the first setting, select the outside of the round stock.
   
4. In order to create the horse shoe shape, we will need a 180deg bend in the bar stock. Set the angle to -180deg, this will place a 180deg bend in the part. (See above image)
5. Next, we need to define how long the straight legs will be.  Set Trim Plane1 and 2 to 3in each. This will move the trim planes to 3in from the two ends of the bar.
   
6. The last setting will be the Triad in the “X” axis, we want to set this to 3in so that the bar will remain oriented correctly to the plane. Click OK to save these settings.
          
7. The result is a horseshoe shaped section of round bar stock. Create another configuration called “unbend” and simply suppress the Flex1feature. Test the configurations.
   Challenge yourself by adding a feature that turns the bar stock to an extruded tube. If done correctly, the part can be converted to a tube that will bend and unbend just like the solid bar.
   

 

Text wrapping is a fairly simple tool to use within Solidworks part modeling when you are applying a wrap to a flat face or around a cylinder, but when you run into a part with a changing radius and a rounded face, the wrap feature becomes a little more complex.  For this example, we will wrap text onto a conical feature.

In order to create  this text wrap, we must first create some construction geometry that is relative to the dimensions of the cone.  By identifying the point where the axis of the cone and the plane of the cone intersect, we can use this point to further create a half circle on our sketch plane.  So lets go ahead and define this point.

Now create a plane tangent to the face of the cylinder; this plane will be used to add the text and text curvature.  You will see that the distance of where the text is placed is going to be the radius of the half circle we create in the next step.  In this example, the text is located 4.7 inches down from the top of the conical section, so go ahead and create a half circle arc with a radius equal to the distance you want the text to be relative to the tip of the cone.

Now all of our construction lines are in place, insert the sketched text and click the arc to create the correct geometry for the text to be wrapped.  Make sure that the text inserted is on the same plane you created but inserted as a different sketch than the construction lines you have created.

Click the wrap feature, choose the sketch of the text you are wrapping and the face of the cylinder and you are all done!

I have always found that the routing tools to be an interesting part of SolidWorks but was never able to really learn all the ins and outs of it. So a while back I started looking a little closer at it. I am right now working from the Piping & Tubing portion of the training manuals.

I always thought the rules for creating the routes were very consistent and that you needed to have connector points (CPoints) and route points (RPoints) to be able create any route. Well I found a tool to be able to start a route without a connector.

This is very helpful if the component you are using is an imported model from a vendor and they supply the connector but you are not sure what it will be. They did let you know the size of pipe/tube/wire and a location for where it will be on the component. So know if it is not all ready on the model you will need to create a cylindrical cut to represent the start point.

The tool to use in this instance is Start at Point and is available on the all three routing tool bars Electrical, Piping, and Tubing. Once you select the appropriate tool you then select the cylindrical face from the hole for the starting point and it gives you a nub start so you can then continue the route in whatever manner you need to complete this.

So as I continue to dive into the routing tools I will add any interesting features that may be hidden or not really well known.

Occasionally you will see SVG output that appears to highlight the entire screen as you mouse over the image. This can be quickly solved by selecting the option: HardwareAdvance.SilhouetteShader. Restart Composer and you should be on your way with improved SVG output.

DID YOU KNOW

You can now tie your Facebook account to the updated and improved  3DVIA Composer forum so that you can easily see the latest activity on the forum through your Facebook feed?