Numeric Sketch Input

In SolidWorks 2009, there was a number of  enhances made to the sketching environment to make your day to day usage quicker and easier. One enhancement to sketches is the ability to specify the numeric input as you create lines, rectangles, circles and arcs. This ability is not turned on by default. You must enable it in the System Options by selecting Options in the Standard Toolbar.

In the System Options tab, select Sketch.

In the Sketch options select Enable on screen numeric input on entity creation.

When enabled, you will have the ability to enter in the value for any of the supported sketch entities. When selecting an entity, for example a rectangle, simply click once to place the rectangle and fields appear for the input of the numeric value. Enter the first number and press Enter or Tab to move to the next field. After adding a value in the second field, press Enter to exit the command or press Tab to return to the first field. This will not place dimensions on the sketch entities, in fact after hitting Enter the dimensions will disappear.

Sketch Dimensions of Zero and Negative Values

Another enhancement to the sketching environment is the ability to specify a zero or negative value for sketch dimensions.  You can imagine how helpful it is to be able to add a zero of negative number to a sketch dimension, especially when using Design Tables and Configurations. In this example, there is a circle in a sketch that is drawn to be 2 inches from a edge on our part. If we wanted to move the circle to the other side of the edge prior to SolidWorks 2009, we would have to delete the dimension and move the circle to the other side of the edge and apply a new dimensions. Now, all we have to do is double click the dimension and add a minus (-) in front of the dimension value and click the green checkmark.

The circle is now on the other side of the edge.

Now if we want the center of the circle to be vertical the the edge, we would normally have to delete the dimension and add a vertical relation to the center and the edge. That works fine but it does cause some problems in multi-configuration parts. Now with SolidWorks 2009, we just double click the dimension and change the value to zero (0) and click the green checkmark.

The circle is now vertically aligned with the edge and the dimension shown in the sketch displays a zero as it value.

Parting Line Analysis

The next enhancement is extremely helpful those who create molded components. This is an enhancement that I was very excited about since I work on a lot on molded components. The analysis tools, Draft Analysis, Undercut Analysis and Parting Line Analysis can now run continuously and report changes as the model is changed. You might be looking at that list of analysis tools and think that something looks different. Well, there is now a new Parting Line Analysis tool added to SolidWorks 2009.

Parting Line Analysis displays a potential parting line based on your direction of pull and changes dynamically as the part geometry is changed.

Magnifying Glass

How many times, when working in a large assembly or part, have you need to zoom in a specific area to do something like take a measurement or edit a small feature. Prior to SolidWorks 2009, you would need to zoom in and out many times but now with the addition of the Magnifying Glass; things have gotten a lot easier. Press G on your keyboard and a circular magnifying glass appears allowing you to zoom in and work on a smaller area of your part. Using the scroll wheel on your mouse you can zoom in and out without effecting the scale of your overall part. Move your mouse around and the glass moves as well, allowing you to work on any feature within the circle.

If you hold the ALT key while using the wheel on your mouse, you can create a section parallel to the screen. When you are done with the magnifying glass you can select G or ESC to close the view.

BOMs in Assembly Documents

Last but not least is the addition of Bill of Materials in an Assembly model. Instead of inserting a BOM into an assembly drawing, you can now add a BOM to the actual graphics area of your assembly model. Select Insert from the menu bar.

Then select Tables -> Bill of Materials.

Just as you would in an assembly drawing, Select the Table Template and any options you want and select the green checkmark.

The BOM will now appear in the graphics area of your assembly providing the same functionality as BOM in a drawing. In fact, when you create an assembly drawing you can insert this BOM into that drawing.

Many More to Come…

This was just a quick description of some of my favorite enahancements to SolidWorks 2009. From now on all the projects, tips and tricks and tutorials will be based on SolidWorks 2009 and we will be able to explore even more enhancements. If you don’t want to miss anything, make sure you subscribe to my RSS feed and I will be back next week with some new content.

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What is SolidWorks World?

Networking Opportunities

Like I mentioned, SolidWorks World is an international user conference and exposition. Probably the best part of SolidWorks World is the chance to meet other users who are just as passionate about SolidWorks as you are. It is the one place where you can proclaim “I am a SolidWorks Geek” without fear. Last year in San Diego, there were over 5,500 SolidWorks geeks meeting for the first time, sharing stories, making contacts and just having fun. In these economic times, having contacts in other companies can be extremely beneficial if the unfortunate happens.

Learning Opportunities

In addition to networking, SolidWorks World provides a unique opportunity to develop your SolidWorks usage skills. With over 150 sessions presented by industry leaders in CAD Administration, Data Management, Design Automation, Design Validation, Education, Modeling Essentials, Productivity Tools, Customer Success/Designing Better Products, Tips and Tricks and Design Communication; there is a wealth of knowledge that will be extremely beneficial to every level of SolidWorks user. In fact I am looking forward to attending the Backdoor Workarounds, Tips and Tricks, and various CAD administration and Data Management sessions.

Learn About New Products and Win!

At the partner pavilion at SolidWorks Works 2009, you can explore the numerous products offered by vendors in the following areas: Analysis/FEM/FEA Software, Component Design/Libraries, Computer Hardware Vendors, Data Translation Software, Design and Drafting Software, Die Design Software, Electrical and Electronics Design Software, ERP/MRP Software, Graphics Accelerators, Implementation/Training, Industrial Design Software, Input/Output Devices, Insp. Reverse Engineering Software, Knowledge Based Engineering, Manufacturing Network, Manufacturing/CAM Software, Mechanical Engineering Software, Optical Design Software, PDM/PLM Software, Processors and Operating Systems, Rapid Prototyping System Vendors, Robot Simulation Software, Sheet Metal Software, Tolerance Analysis Software, Utilities and Viewing, Rendering, and Collaboration.

While you are exploring the partner pavilion, you can get a game card that the various exhibitors will stamp when you visit with them. After collecting 16 stamps from different exhibitors you can win some prizes and all those who complete their game card will be entered into a drawing to receive a $1000 American Express® Gift Cheque. How cool is that? Even without the prizes, exploring the many products offered is fun. It is always my favorite part of any conference I attend.

Speakers

Every year at SolidWorks World there is always a buzz about the speakers. This year is no different. In addition to the keynote speeches by Jeff Ray, the CEO of Dassault Systèmes SolidWorks Corporation and Jon Hirschtick, the Co-Founder and Group Executive of Dassault Systèmes SolidWorks Corporation; this years guest speaker will be Sir Richard Branson, the Founder and President of the Virgin Group. If you are not familiar with Sir Richard Branson, check out his Wikipedia entry. I am personally very excited about seeing him in person. Being the space and astronomy junkie that I am, I am hoping to hear about his venture Virgin Galactic.

Register Now!

This was just meant to be a quick introduction to SolidWorks World and I hope you are excited about going. If you haven’t already done so, make sure you register by following this link. If you register before January 9th, 2009 you will receive a discount.

I am extremely excited about attending my very first SolidWorks World and I hope I will be able to meet as many of my readers as possible. Over the next few months leading up to SolidWorks World writing more about the event. So make sure you stay tuned, if you’re interested you can also follow the SolidWorks World buzz on twitter.

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Finishing up the Cradle Model

The next feature, is the cut out that the staples will pass through when the stapler is in use. As the staples are fed down the cradle, they will be individually pass through this opening and formed with the anvil.

1. Select the top face of the cradle and click Insert Sketch in the Context Menu.
2. Press ‘S‘ on the keyboard and select Line from the Shortcut toolbar.
3. Starting at one of the inside corners, roughly sketch out the shape shown below.
4. If you didn’t do so when creating the sketch, make the various points and lines Coincident and Collinear with the edges of model by selecting and sketch entities and edges while holding CTRL. Then select the appropriate relation in the PropertyManager.
5. We need to make the sketch symmetrical, instead of using construction lines, we are going to achieve this with relations. First, select the two line segments labeled “a” while holding the CTRL key and select the Equal relation from the PropertyManager.
6. If all of the other sketch segments are either horizontal or vertical, There is no need to make the two segments labeled “b” equal. Instead, select both segments while holding CTRL and select the Perpendicular relation from the PropertyManager (The relations can also be selected in the Context menu)
7. The last relations we need to add will be to the segments labeled “c“. Select both of the “c” segments and select the Equal and Collinear relations from the PropertyManager.
8. Next, press ‘S‘ on the keyboard and select Smart Dimensions from the Shortcut toolbar.
9. Place the .038″, .063” and .075″ dimensions as shown below.
10. Select Extruded Cut from the Features toolbar.
11. Change the End Condition for Direction 1 to Through All.
12. Click the green check mark.

Now we need to cut out a corner relief for when we convert the part to sheet metal and while we are at it, it is also a good time to make clearance for a future component.

1. Select the front face of the cradle and select Insert Sketch from the Context Menu.
2. Press ‘S‘ on the keyboard and select Corner Rectangle from the Rectangle fly-out in the Shortcut toolbar.
3. Starting at the lower-left corner of the face, draw a small rectangle and do the same of the lower-right corner.
4. Press ‘S‘ once again and select Center Rectangle from the Rectangle fly-out in the Shortcut toolbar.
5. With the center of the rectangle near the middle of the part, draw a rectangle approximately where shown.
6. Before we can start placing dimensions we should add as many relations as possible to the sketch. First, select the top line of the center rectangle and the top edge of the part while holding CTRL on your keyboard. Then select, the Collinear relation from the PropertyManager.
7. Select the centerpoint of the rectangle and the sketch origin while holding the CTRL key and select the Vertical relation from the PropertyManager.
8. Select the two top segments, of the lower two rectangles while holding the CTRL key and select the two relations Equal and Collinear from the PropertyManager.
9. Now it is time to add those dimensions. Press ‘S‘ on the keyboard and select Smart Dimensions from the Shortcut toolbar.
10. Make the top rectangle .165″ wide by .090″ tall.
11. Since we made the top segments of the two lower rectangle Equal and Collinear, we only need to add a couple of dimensions. First, make the height of one of the lower rectangles .045″. Then make the distance between the two .450″.
12. The sketch should now be fully defined, if not you need to go back and make sure you added all of the appropriate relations.
13. Select Extruded Cut from the Features toolbar.
14. Change the End Condition of Extrusion 1 to Up to Surface and select the highlighted surface below. This is the face we created in the cut feature earlier.
15. Click the green check mark.

We are almost done with adding all of the features. All that is left to do is add two holes on the bottom surface of the cradle. Once again, I am not exactly sure as to the purpose of these features. My best guess is that that are used by a fixture during the assembly process.

1. Select the face on the bottom surface of the cradle and select Insert Sketch from the Context menu.
2. Press ‘S‘ and select Center Circle from the Circle fly-out in the Shortcut toolbar.
3. Draw two circles, approximately where shown, on the surface.
4. While holding the CTRL key, select the center of the circles and the sketch origin.
5. Select the Horizontal relation from the PropertyManager.
6. Select both circles while holding the CTRL key and select the relation Equal from the PropertyManager.
7. Once again, Press ‘S‘ on your keyboard and select Smart Dimensions from the Shortcut toolbar.
8. Select one of the circles and make the diameter .156″
9. Select the right edge of the part and the circle on the right. Enter the dimension value of 1.700″.
10. Select both circles and make the distance, between them, 3.250″
11. Click Extruded Cut from the Features toolbar and change the End Condition of Direction 1 in the Extrude PropertyManager to Up to Next.
12. Click the green check mark.

The actual part is now complete. We can now convert the part into a sheet metal part.

Converting Solid Model to Sheet Metal

In the Sheet Metal toolbar, select Insert Bends. If you do not have the Sheet Metal toolbar in your CommandManager, right-click one of the tabs and select Sheet Metal.

The first thing we need to do is specify the fixed face of the model. Imagine that you placing this part in a fixture, this is the face that you will be clamping down when you bend the part down to make a flattened pattern.

In the model, select the bottom-inside face of the part.

Set the Bend Radius to be .015″. This value will vary depending on your parts you are trying to bend. Sometimes you may encounter errors when trying to create a sheet metal part from a solid that can be remedied by playing with this value. Click the green check mark.

Looking in the FeatureManager, you will now see three new features for the sheet metal part. The first feature, Sheet-Metal4, makes the part a sheet metal part. The next feature, Flatten-Bends4, creates a flattened version of the converted part. The last feature, Process-Bends4, bends the flattened pattern back into a sheet metal form.

Add Forms to Side of Cradle

Now that we have converted the part into a sheet metal component, we can use sheet metal forms to complete the part. In the attached zip file(Staple Cradle, Stapler (67)), you will find the form that you need to use for this model. Place the form in your Sheet Metal Forming Tools folder in your design library. If you do not know how to do this, you can go here for more information.

1. Drag the Staple Cradle Form Die from the Forming Tools folder in the Design Library directly onto one of the inside faces of the cradle.
2. Press ‘S‘ on your keyboard and select Smart Dimensions from the Shortcut toolbar.
3. Make the vertical construction line 2.950″ from the outer edge of the part and make the horizontal construction line .198″ from the top edge.
4. Click the green check mark.
5. Repeat steps 1-4 for the other inside face of the cradle.

The staple cradle is now complete and ready to go into your assembly.

Wow… That Was Long…

Well, it took a few days but I finally managed to finish this post, thank you for sticking in there. Let me know what you think about the new approach to my tutorials. They take a little longer to write but they are meant to give you, the reader, the whole story. Ciao!

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Create Model of Staple Cradle

Create the base feature for the staple cradle. All of the subsequent features will be added or removed from this base feature.

1. Create a sketch on the Top Plane.
2. Click Center Rectangle in the Sketch toolbar.
3. Place the center of the rectangle on the origin of the sketch.
4. Press “S” on keyboard and click the Smart Dimensions button on the Shortcut toolbar.
5. Using Smart Dimensions, make the rectangle 5.700″ long by .595″ high.
6. Click the Extruded Boss/Base button in the Feature toolbar.
7. Make sure the End Condition Type is Blind.
8. Make the depth (D1) .565″.
9. Click the green check mark.

Cut the top of the created extrusion. This is to achieve the basic shape of the top of the staple cradle.

1. Select the side surface of the extrusion.
2. Click Insert Sketch in the Context Menu.
3. Press ‘S‘ on the keyboard and click Line in the Shortcut toolbar.
4. Select the top corner of the face and trace out the profile shown closing on itself.
5. Press ‘S‘ on the keyboard and click Smart Dimensions in the Shortcut toolbar.
6. Make the distance from the bottom edge of the face to the bottom line of the profile .450″.
7. Make the angle of the segment on the right side of the profile 60° off of the top line.
8. Make the right most point of the profile .825″ from the right edge of the face.
9. Click the Extruded Cut button in the Features toolbar.
10. In the Extrude PropertyManager, change the End Condition of Direction 1 to Up To Next.
11. Click the green check mark.
    

Shell out the part to create the basic shape of the staple cradle. After this step the model is beginning to look more like the staple cradle.

1. Select Shell from the Features toolbar.
2. In the Shell PropertyManager, set the thickness in the field labeled D1 to be 0.040in.
3. Select the Faces to Remove field in the Shell PropertyManager.
4. Select the four faces shown below. These faces will be removed when the feature is shelled out.
5. Click the green check mark.

Now this is starting to take shape.

Now we need to create the tail end of the part. This is where the rivet will tie many of the pieces of the stapler assembly together.

1. Click the side face of the part.
2. Select Insert Sketch in the Context Menu.
3. Click ‘S‘ on your keyboard and select Line in the Shortcut toolbar.
4. With the Line tool active, click the bottom edge of the face about a half an inch from the left edge.
5. Draw a short line vertically and a second segment to the left horizontally.
6. Press “A” on your keyboard to activate a tangent arc from inside the line command.
7. Click the upper edge of the face.
8. Hold the ‘CTRL‘ key on your keyboard while selecting the arc and the left edge of the face.
9. Select the Tangent relation in the PropertyManager.
10. Hold the ‘CTRL‘ key on your keyboard while selecting the arc and the top edge of the the face.
11. Select the Tangent relation in the PropertyManager.
12. Press the ‘S‘ key on your keyboard and select Smart Dimensions in the Shortcut toolbar.
13. Make the right segment in the sketch .450″ from the left edge of the face.
14. Make the bottom segment of the sketch .045″ from the bottom edge of the face.
15. Click Extrude Cut from the Features toolbar.
16. Since this is an open sketch, the only option we can change in the direction of cut. Look at the direction indicated with the small arrow near the bottom of the sketch. This indicates the direction that the feature will make the cut. If the other direction is desired, select Flip Side to Cut in the Extrude PropertyManager. Do it now and you will see the arrow flip directions.

Now we need to create the hole for the rivet.

1. Select the face and click Insert Sketch from the Context Menu.
2. Press ‘S‘ on your keyboard and select Center Circle in the Shortcut toolbar.
3. Hold the ‘CTRL‘ key on your keyboard and select the arc edge on the face and the circle you sketched.
4. Select Concentric in the PropertyManager.
5. Press ‘S‘ on the keyboard and select Smart Dimensions in the Shortcut toolbar.
6. Make the diameter of the circle .156″.
7. Click Extruded Cut in the Features toolbar.
8. Change the End Condition to Through All.
9. Click the green check mark.

When the stapler is assembled, the following cut will be used to snap another sheet metal into place.

1. Select the side face of the part and select Insert Sketch from the Context Menu.
2. Press ‘S‘ on the keyboard and select Corner Rectangle in the Shortcut toolbar.
3. Create the rectangle approximately where shown.
4. Press ‘S‘ and select Smart Dimensions from the the Shortcut toolbar.
5. Make the bottom edge of the rectangle .145″ from the bottom edge of the face.
6. Make the height of the rectangle .155″
7. Make the left segment of the rectangle .100″ from the left edge of the face.
8. Make the width of the rectangle .100″
9. Select Extruded Cut from the Features toolbar.
10. Change the End Condition in the Extrude PropertyManager to Through All.
11. Click the green check mark.

The next feature, I must admit, I have no idea what it is for. My best guess, is that allows you to see if there are any staples in the cradle.

1. Select the face of the the part and click Insert Sketch in the Context Menu.
2. Press ‘S‘ on the keyboard and select Line from the Shortcut toolbar.
3. Draw a short diagonal line
4. Press ‘S‘ and select Offset Entities in the Shortcut toolbar.
5. Select the line that you sketched.
6. In the Offset Entities PropertyManager, set the offset distance to .045″.
7. Select Add dimensions in the Offset Entities PropertyManager.
8. Select Select chain in the Offset Entities PropertyManager.
9. Select Bi-directional in the Offset Entities PropertyManager.
10. Select Make base construction in the Offset Entities PropertyManager.
11. Select Cap Ends in the Offset Entities PropertyManager.
12. Select Arcs in the Offset Entities PropertyManager.
13. Click the green check mark in the Offset Entities PropertyManager.
14. Press ‘S‘ on your keyboard and select Smart Dimensions in the Shortcut toolbar.
15. Make the two centerpoints of the slot .205″ and .320″ from the top edge.
16. Make the two centerpoints of the slot .370″ and .500″ from the right edge.
17. Select Extruded Cut in the Features toolbar.
18. Change the End Condition in the Extrude PropertyManager to Through All.
19. Click the green check mark.

More to Come…

I think that will do it for today, I find if the articles get way too long people eyes glaze over. Part two of this article will be tomorrow morning at the latest.

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Finishing the Bottom Half

Now that part has been split, we will no longer be needing the radiated surface. We cannot delete it because it would cause our split feature to fail. Instead, we must hide it from view by selecting the surface and clicking Hide in the Context Menu. You will be able to find the surface for future use in the Surface Bodies folder in the FeatureManager.

Now, we are going to be adding a lip for mating on the bottom half of the egg. In order to get to the bottom body, we are going to hide the top half from view by selecting the top half and clicking Hide from the Context Menu.

The bottom half of the egg can now be finished by extruding a lip from the face that was created by the split.

Create an extrusion from the face of the split that is .030″ thick from the inside edge extruded .050″ high.

1. Select the face of the split egg and create a sketch.
2. Select the inside edge of the face and select Convert Entities from the Sketch toolbar.
3. Click Extrude Boss/Base from the Features toolbar.
4. Set the Extrusion Depth to be .050″ from the face of the split.
5. Select Thin Feature in the PropertyManager and enter the Thickness to be 0.030″.
6. Click the green check mark.

Hiding and Showing Solid Bodies

With the bottom half finished, you need to switch the solid bodies that are visible. In the Solid Bodies folder, you can see the two solid bodies we created earlier. The shaded icon represents a visible body and the outlined icon means the body is hidden.

Click on the visible body in the Solid Bodies folder and click Hide in the Context Menu.

Then select the other body and click Show in the Context Menu.

Finishing the Top Half

Since the lip on the bottom half of the egg was an extruded boss, we will need to create a cut on the top half of the egg.

Create an cut extrude from the face of the split that is .030″ thick from the inside edge extruded .050″ deep.

1. Select the face of the split egg and create a sketch.
2. Select the inside edge of the face and select Convert Entities from the Sketch toolbar.
3. Click Extruded Cut from the Features toolbar.
4. Set the Extrusion Depth to be .050″ from the face of the split.
5. Select Thin Feature in the PropertyManager and change the type to Two-Direction.
6. Set Thickness1 and Thickness2 to both be .030″.
7. Click the green check mark.

With the half finished, show both of the solid bodies. If you section the egg longitudinally, you can see the two halves and how they fit together.

Saving Solid bodies Externally

With the two halves of the egg completely modeled, we can save the parts externally. To save the parts , click Insert -> Features -> Save Bodies.

In the Save Bodies PropertyManager, you will see the two newly created bodies listed in the Resulting Parts section.

To specify the path and filename for the two bodies, double-click the first file in the Resulting Parts section.

In the Save As window, specify the location and filename for the first part.

Do the same for the second part.

In the graphics area, the individual parts will be highlighted pink and the callouts will display the full path for each part.

The files listed in the Resulting Bodies section will also be updated to display the name you specified in the Save As window. Click the green check mark and the files will be created and saved externally.

In the FeatureManager a new feature for the Save Bodies is displayed. If you delete or modify this feature, the externally saved parts will be effected.

In the new files, the FeatureManager shows how the the part is externally linked to the parent model. As with Derived Parts, Any changes made to the child part will not be reflected in the parent but changes to the parent part will update the child.

Eggs-ellent Tool!

Hopefully, if you tend to design many plastic parts you will find this technique helpful. Also, if you seen the original video you will notice that I followed different steps to achieve the same outcome. This should illustrate that, in SolidWorks, there are more ways then one to do anything.

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Using the same egg model, Egg Models (167), we are going to try a different approach.

Creating the Egg Shell

The first thing we are going to do this time is shell out the egg model. Click Shell in the Features toolbar.

Set the wall thickness to 0.060″ and since this is a complete body that we will split later, there is no need to select a face to remove.

Adding a Split Line

Now we are going to create the split line that we will use later to determine where the split will take place. The split line will not split the part instead it splits the selected surface on the model. Click Split Line in the Mold Tools toolbar. If the Mold Tools toolbar is not shown in your command manager, right-click a tab on the CommandManager and select Mold Tools from the menu.

If you have used the Split line command before, you know you can project a sketch onto a surface to split it. This time we are going to try something different. By selecting the Silhouette option for the Type of Split, we will create a split line at the largest part of a cylindrical surface. This will ensure that the part will be split at the most logical location for molding.

The Direction of Pull is the direction that the mold will be pulled off of the part when it is being made. After selecting the field you must then select a plane or face that will indicate the direction of pull perpendicular to the selected face.

In the Fly-out FeatureManager, select the Right Plane since it is the plane that is perpendicular to the direction of pull.

The plane that indicates the direction of pull will be indicated with Pink in the graphics area.

Next, the Faces to Split field must be selected in the PropertyManager.

In the graphics area, select the face on the model to be split. The face will be highlighted in blue.

Looking at the side view, the split line does not actually fall in line with the plane that was selected for the direction of pull. Instead, the split line was automatically created at the largest part of the face to ensure there is no undercut.

Create a Radiate Surface

Using the split line we created, we will create a surface that radiates from the model that we can then use to split the model. In the Mold Tools toolbar, select Radiate Surface.

In the Radiate Surface PropertyManager, select the Radiate Direction Reference field. The surface will not be created on the selected surface or plane but instead will run parallel to it.

Once again, select the Right plane in the Fly-out PropertyManager. If your planes are visible, you can also select the plane in the graphics area.

In the PropertyManager, select the Edges to Radiate field. This will be the edge that will be used to create the radiated surface.

In the graphics area, select the split line we created earlier.

The only option that we are concerned about here is the distance that the surface will radiate from the surface of the part. The actual distance does not matter for this case, so accept the default value shown. In case your wondering, if you select the Propagate to tangent faces option, the connected edges on tangent faces will also be selected to create the surface. Since we only have one edge, we do not need to select this option.

The surface now extends from the face of the model to the specified dimension.

Splitting the Egg

With our surface created, we can now split the model into two separate solidbodies. Select Insert -> Features -> Split.

In the Split PropertyManager select the Trimming Surfaces field. This is the surface, or sketch, that is used to split the model.

In the graphics area, select the surface we created using the Radiate Surface command.

Next, select Cut Part.

In the Resulting Bodies field, select the bodies that will be split. If you keep a check box clear the body will not be split and it will remain with the original part. Since we only have two bodies, this is not important to us but if we had multiple bodies that would be created with the split we can select which bodies will be separate.

In the graphics area, the Resulting Bodies will be identified with a callout and the bodies will be shown in pink. The Trimming Surface will be shown in blue. Click the green check mark and the model will be split.

In the FeatureManager, the split feature will be shown and you can edit it later if needed.

In the Solid Bodies folder in the FeatureManager, the newly created bodies are shown.

We’re Not Done Yet…

That’s it for today, later in the week we will finish our little easter egg. We still need to create the lips and save our model so make sure you come back.

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Today’s example will be making modifications to a purchased die set that can be purchased from many vendors. If you aren’t familiar with die sets, they are handy kits that usually contain a couple of pre-machined plates, shafts and bushings. They are a great time saver when you create tooling for a variety of uses.

Inserting a Part

To start off, open a new part in SolidWorks. From the Insert menu, select Part.

In the Open window, select the part that the new part will be derived from.

A representation of the referenced part will be shown in you graphics area.

In the Insert Part PropertyManager, you can select the elements of the original part you want to transfer into the derived part. You can add as few or as many elements but I tend to go with the minimalist approach and transfer only what I know I will be using at a later time. At this point you can select the Launch Move dialog option in the Locate Part section to locate the inserted parts in relation to existing sketches or part geometry. Since this is the first feature we are adding to the part, click the green check mark and the part will be inserted in the orientation it exists in the original part.

You will now see the part shown as a feature in the FeatureManager followed by a arrow (->) this designates that the feature has an external reference.

Expanding the feature will show you the elements you selected to be transferred into the new part.

Locating Inserted Part

We will be covering locating a part in the future when we discuss multibody parts but I wanted to show you the Locate Part command. If you select the Launch move dialog…

…you will be presented with a PropertyManager that same basic mates used in assemblies to locate your solidbodies.

Add Features to Inserted Part

Once the referenced part has been inserted into your derived part it becomes a solidbody. You can add features to the part just like any other solidbody but you cannot not modify any of the existing features of the referenced part. In this example, I wish to add a series of holes that will be used as mounting for another part.

You will see in the FeatureManager, that the holes I added are a new feature in the derived part and the original solidbody has not been changed.

Breaking Link to Referenced Part

As I mentioned, you cannot modify the features of the referenced part. If you needed to make a change to the parent part, you must modify it separately but understand that any changes made to the parent part will be reflected on all of the derived parts made from the parent part. If you need to modify the features of the part only in your current model and you do not wish to affect any more of your parts; you can break the link to the parent and transfer the model information into you current model. To do this right-click the feature in your FeatureManager and select List External Refs.

In the External References window you will see the external references to the part part listed, as well as any other external references you may have created in you part.

In SolidWorks 2008, a new option was added that allows you to insert the features from the parent part when the references are broken. Select Insert the features of original part(s) if references are broken.

Then click the Break All button.

You will be prompted with a message warning you about breaking the references and how you will not be able to undo the action. Select OK.

The external references list will now be clear and the features from the original part will be inserted into your FeatureManager under a new folder that contains the name of the original part. You can leave the features in the folder or delete the folder if you prefer it.

In addition to breaking the links after the part is inserted you can also choose to break the link when the part is inserted by selecting Break link to original part in the Insert Part PropertyManager.

This can be buggy at times

Just a warning about breaking the links to the original part. I have found that in SolidWorks 2008 that sometimes SolidWorks will crash when you try to break the link to some parts. In fact, in writing this article I was unable to break the link to my part without my SolidWorks crashing on two separate computers, that is why I do not show the FeatureManager after the part link is broken. I have not had the opportunity to test this out in SolidWorks 2009 yet and I hope that it has been addressed. Let me know what you experiences are with breaking the link to external parts.

More to Come…

That does it for today’s introduction to inserting parts to make derived parts. Soon we will be looking at the other two types of Derived Parts: Mirror Part and Derived Component Part so make sure you subscribe to my RSS feed so you don’t miss anything. Ciao!

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Creating a Derived Sketch

For today’s example I am using a model I threw together just to illustrate the function. The actual geometry is not important here, just the process being described. Here we have a cut out on one the surfaces that we would like to replicate elsewhere on the part.

In the FeatureManager, select the sketch that makes up the feature.

Then, while holding down the CTRL key your keyboard, select the face (or plane) where you will be placing the sketch.

After selecting the sketch in the FeatureManager and selecting the destination while holding the CTRL key, select Derived Sketch from the Insert menu.

A new sketch will be created that is derived from the parent. If your expecting some kind of confirmation, you will not see one. The only indication you will see is that a new sketch is shown in the FeatureManager followed by the word ‘derived‘. The new sketch will be created directly over the parent but it will be blue since it is not fully defined.

Using your mouse, drag the derived sketch to the intended location on the part. The derived sketch cannot be modified except for it’s position and orientation using dimensions and relations. In fact, you may notice that every tool in the Sketch tool bar is grayed out, this is because you can not even add any sketch elements to the sketch.

All that is left to do is to create your feature from the derived sketch. For this example, we are going to create another Cut Extrude just like the parent feature.

Modifying the Parent Sketch

The best part about using derived sketches it that, unlike when using Convert Entities, you can add, remove and modify entities in the parent sketch and ALL the child sketches will be updated. Take for example the part we have been working on, this peanut shape sketch was just not what I was looking for. Instead, a regular hole would be better suited for this feature.

I can edit the sketch and delete every entity and add all new entities. I must stress here that I said “edit the sketch” and not delete the sketch, deleting the sketch will break the references to the derived sketches.

Upon leaving the sketch, all of the derived sketches have been updated.

Creating Derived Sketch at Different Heights

Derived sketches do not need to be on the same plane, or elevation, as the parent sketch. In fact, the derived sketches don’t even have to share the same orientation as the parent. If the intended face, or plane, is a different elevation; select the face, just as before, while holding down the CTRL key and select Derived Sketch from the Insert menu.

This time when the derived sketch is created, it is in line with the parent sketch but it is not on the same elevation as the selected face. As before, drag the newly created derived sketch to it’s intended location and apply the necessary constraints.

Do another Cut Extrude, and you have a huge time saver.

Deleting the Parent Sketch

I mentioned earlier about deleting the parent sketch of derived sketches. If you attempt to delete a sketch that has derived sketches, they will not be deleted. Instead that will be “underived“, as the message states, and will discuss that further in the next section. If you attempted to delete the sketch by accident, click No and the command will be canceled.

Underiving a Sketch

There will be times when your derived sketch must step out on its own and become it’s own sketch. Everything was fine when the parent sketch was calling the shots but now it is time to modify a derived sketch independent from it’s parent. Underiving a sketch breaks any relationship to it’s parent sketch and allows you to make modifications to the sketch. In the FeatureManager, right-click the derived sketch and select Underive from the menu.

The word “derived” will no longer follow the sketch name and you may continue to changes to the sketch.

Where Have You Been All My Life?

I bet your thinking of instances in the past where using Derived Sketches would have been extremly helpful. When I first learned about Derived Sketches, I wished I could go back and redo many models but I have since made up for time lost. I am sure your already thinking a ways you can use Derived Sketches on your current project. Have fun with it!

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