I had made this model just for fun and wasn’t planning on using it in the blog, but I’ve got so many requests for instructions and files that I ended up writing a short tutorial for it.  Hope it’s useful for someone out there. The files were all made in SolidWorks 2010.

To download the files and pdf document, click on the following links. I’m also adding links to these documents in the downloads  page.

Scissors Tutorial (pdf)

Scissors SolidWorks files (2010)

He began by showing us some common ways to do modifications in the geometry of an imported part. As you know, usually when you import a part -step, parasolid, iges, etc-  you are not going to have access to its features to modify any dimensions. Since all you usually have is an imported feature (dumb part) or imported surfaces,  it’s common practice to do modifications via the “Butcher Approach”, as Michael calls it, and that is basically slashing, moving and  then reconnecting and patching parts of the geometry.  He demonstrated this approach through an example.

Michael started with a step file that he opened in SolidWorks. After running import diagnostics and healing a couple of faces, we had no features on that tree. Michael used the “Butcher Approach” to make the legs of this part you see here  a little longer. First, he began by slashing the model using a line that was sketched on the Front plane and the Split command (Insert, Features, Split). This way, he cut the model in three solid bodies: the frame and two of its legs. They are all in the same color in the image, but you can see there’s actually three bodies and each one has a callout right next to it.  The three solid bodies will appear in the Solid Bodies folder in the Feature Manager tree.

Next, he used Move/Copy Body  (Insert, Features, Move/Copy Body)  to translate both legs down by 20 mm. Note that Move/Copy Body also has the option of using constraints. We don’t want to use constraints, so make sure to choose Translate/Rotate under options in the Move/Copy Body property manager. You will see a Triad appear. You can use this triad to dynamically move the bodies down by dragging the green arrow, or you can enter numerical values for the new position directly from the property manager on the left.

By now, both legs have moved down and now there’s a gap that needs to be filled.

Michael used the Boundary Boss feature to fill the gap and reconnect the bodies. He could’ve also used loft or even a surfacing technique, but Boundary Boss did the trick this time.  So there you have it, the Butcher Approach.

Next, he showed us a direct modeling approach, using Move Face. First, we needed to turn on the Direct Editing Command Manager tab by right clicking on any of the other tabs and selecting Direct Editing from the list.

He used Move Face to translate those six faces you see here ten millimeters towards the inside of the leg. Notice that we needed an edge to specify the direction of translation, so we used the one you see highlighted there next to the pointer. The preview of the new location appears in yellow.

Something important: Once we accept the Move/Face feature, it will show up in the Feature Manager as an other feature that can be edited, but not only that, we can now use Instant3D to dynamically drag a face in this leg, for instance, as you see in the image below. Notice that dragging the face with Instant3D doesn’t add another feature to the tree because, in fact, every time you drag the face using Instant3D you are simply editing the Move Face feature that had been added previously.

Move Face can also be used to offset a face in a body, like you see in the following image. Here, Michael instructed us to offset the face highlighted in blue 1 mm towards the part. Once we accept the feature, all other faces around it will be modified accordingly and, just as before, we’ll be able to use Instant3D to dynamically drag this face.

There’s also an option to rotate the face instead of moving it or offsetting it. To use this option we need to specify an axis for rotation and an angle. In this image, the vertical edge on one side of the face was used as the axis and we rotated the face 15 degrees from its original position.

Notice that once we accept the Move Face feature the hole doesn’t show up in the face we just rotated, but that all the rest of the geometry has changed accordingly and the hole now shows up going through other faces in the part.

Michael corrected this situation by using Move Face again to translate the geometry associated with the hole. Notice the edge of the face that is used to specify the direction of translation. The preview of the new location shows up in yellow.

He also demonstrated the use of this technique in a large model when he used Move Face to change the location of some of the support ribs on this engine block. By the way, those ribs are not really part of a pattern, but Michael did mention that Move Face can be used to change the location of one, two or more instances inside of a pattern without disturbing the rest of the pattern.

He first changed the model to a Right side view and Wireframe display style to make it easier to select the geometry. He used Move Face command again to translate the faces of two of the ribs. He selected the faces associated to the ribs  by dragging a box from left to right as you see in this image.

Once the faces were selected, he used a horizontal edge in the part to specify the direction of translation and moved the geometry 2 in to the right. It’s a bit hard to appreciate in this image, but there’s a preview of the new location of the ribs. The lines in blue are the ribs in their original position, and the preview shows up in yellow.

Michael also showed us how to use FeatureWorks to recognize features in an imported part. This can be done locally, by right clicking on a face, for instance, and selecting Edit Feature from the flyout toolbar. FeatureWorks then will recognize features such as extrudes, holes, revolves, etc. that could be associated with the geometry selected. We can also recognize features in the whole model at once by right clicking on the imported feature in the Feature Manager tree and selecting FeatureWorks, Recognize Features, as you see in the following image.

FeatureWorks will then recognize features such as extrudes, revolves, holes, ribs, fillets, etc. and create a Feature Manager tree for the part. This can save some time and effort. For instance, after recognizing features in this imported part, I suppressed the ones that were associated with the engraved plate.

I believe the complete presentation with files and step by step instructions will be available in March. Until then, as usual, I hope my brief chronicle was useful for someone out there.

Thanks to Michael LaFleche for a great hands-on presentation. I really enjoyed it.

Anyway, I’ve also been spending some time exploring SolidWorks 2010 Beta,  preparing for my presentation at my local user group (although I just learned it’s been changed for September), getting ready for a couple of trips (travelling with dogs is complicated), and answering old and new email that has been accumulating.  One of those emails inspired this post.

A reader had a problem trying to create something like a spring. I know, you can make that easily with a helix and/or a sweep, right? Yes, but the tricky part was that he needed the ends of the spring to bend towards the axis of the spring.  I wasn’t quite sure at first what he wanted to do, so I referred him to a couple of tutorials from Matt Lombard’s SolidWorks 2007 Bible that I remembered going through a while ago. In one of them a spring with a little hook attached to one of its ends is modeled using projected and composite curves. The other one is a helical sweep where the profile appears to grow larger as it travels along the helix. Just as I was getting proud of myself for saving those old files “just in case”, he wrote me back saying the tutorials were good, but he still couldn’t find the way to do what he needed to do. He sent me a picture (that I won’t publish here) and the practice part he was working on, and my first thought was to start fixing the sketches for the projected curve he needed, but after taking a closer look to those pictures, it occurred to me that what he was really trying to do could actually be accomplished in a much simpler way, just by taking better advantage of what splines and 3DSketches have to offer.

See, you start with a circle centered on the origin and a simple helix, not tapered and constant pitch. I only needed one revolution or so for this one, but that’s not really important.

Next, you are going to open a 3DSketch, select the helix and convert it into the 3DSketch by using Convert Entities. See, unlike what happens when you convert a helix into a sketch, where you end up with a projection of the helix on the sketch plane, when you convert a helix into a 3Dsketch, you end up with a sketch entity that is just like the helix you had before, all 3D and no flat, it’s actually a spline, and you can drag the ends and add other entities and relations inside the same 3DSketch, as well.

My reader needed the ends of the helix to go back to the center.  Imagine a wire that runs vertically along the axis of the helix, then bends around to form the spring and comes back to the center to continue running vertically along the axis. That’s what he needed.  In order to do that, and still inside the same 3DSketch, change to a Front view and sketch a vertical line along the Y axis. You should see the relation AlongY added to this line, if you don’t have it, add it through Display/Delete Relations, Add Relation.  Also add a coincident relation between this line and the origin.

Still inside the same 3DSketch, change to an isometric view, or at least rotate the view a bit so you can see better what’s going on, and sketch a two point spline joining one of the ends of the helix with one of the vertical lines. At first, the spline will look like it’s just a line, but you can make it look curvy by dragging the handles.  Select the spline and the helix and add a relation (Display/Delete Relations, Add Relations). This relation can be tangent or equal curvature, whichever works better for your purposes.

Now, in order to smooth out the transition from the spline to the vertical line, select both the spline and the vertical line and use Tools, Spline Tools, Fit spline, to fit both entities into one single spline.  Make sure the option to close the spline is unchecked.

Notice that you can still adjust the transition even more by dragging the spline handle, like in this image.

Then you simply use this 3DSketch as the path for the sweep and that’s it. No need for complicated ways for this one, just to remember what can be done with the tools we have.

I wanted this vase to be just like one my husband gave me a few years ago, and that unfortunately broke. Although basically squared shaped, the walls of the vase are somehow curvy, so I began by creating a surface extruding an arc sketched on the Top plane, as you can see in the following image.

After that, I created an axis (Axis1) between two points in the lower edge of the surface. The idea was to use this axis to rotate the surface around it a few degrees, since the walls of my vase don’t precisely go straight.  For this purpose, I used the command Move/Copy Bodies, but only to rotate the surface, not to copy it. In the image you can see the selected surface in blue and its new position in a pale, almost transparent, shade of yellow.

The rest of the walls for the vase were created by patterning this first wall around Axis2, which is an axis I created in the intersection of the Front and Right planes. Notice that all these “walls” are simply surfaces that intersect each other and still need to be trimmed.

I trimmed the four surfaces against each other using the Trim Surface command. By selecting Mutual as the trim type, not only the four surfaces get trimmed as well as work as trimming tools themselves, but the result is also knitted together as one surface body in the end.  The purple faces are the ones that are being kept.

Next, I created a plane that goes through Axis2 and one of the top vertices of the vase. In this plane, I sketched a profile to help me model the top of my vase.

I wanted to create a surface by sweeping a sketch (the profile) using the upper edges of the vase as my path, only  problem is that these edges  do not rest in one plane, so what I did was to open a 3DSketch (Insert, 3DSketch) and convert those edges. Once I had my profile and path, I used the command Sweep Surface, as you can see in the following image. The swept surface is shown as a preview.

My vase has some indentations on the walls, and I wanted to recreate them.  With this idea in mind, the first thing I did was to offset one of the walls to the inside of the vase. It’s is hard to appreciate it, unless I hide the other faces, but maybe you can see the offset surface in the detail of the preview. It’s the one shaded in pale yellow.

I created a sketch on the front plane by offsetting the edges of the vase wall and used it to trim two of the four faces of the vase, the one directly in front of the Front plane and the one behind it. In the image, the surfaces in purple are the ones being kept.  Next, I created the same sketch in the Right plane and used it to trim the remaining two faces.

Once again, on the Front plane, I created a sketch by offsetting the one created in the previous step to the inside. I used this new sketch to trim the offset surface I had created previously. The part in purple is the one I’m keeping.

I used the Boundary Surface command to create surfaces to connect the wall of the vase to the trimmed offset surface, like you see in this image.

I did the same for the rest of the edges and then patterned all five surfaces (the trimmed offset surface included) around Axis2, as you see in the image.

At this moment, I had a total of twenty two surface bodies, so I decided to knit them together, using the Knit Surface command, but I didn’t try to form a solid just yet. After using the Knit Surface command, I had only one surface body in my folder.

If you look at it closely from the front or from the right, you will notice that the bottom of the vase is not really flat, so what I did was to trim the bottom using the Top plane as my trimming tool.  Once the bottom was flat, I was able to use the edges to create a planar face to close the vase at the bottom using the Planar Surface command. I knitted this new surface and the one I already had together afterwards.

Next, I applied a few fillets to soften the edges of the vase, and finally, used the Thicken command to make it into a solid by adding thickness to the surface. Notice that this is working for all these surfaces at once only because they are knitted together. You can add thickness to the outside, the inside, or to both inside and outside at the same time. In this case, I decided to apply the thickness to the inside of the vase.

So there you have it. It’s not perfect…

I’m still not so happy about how the fillets look like. The upper edge in particular seems to be extremely hard to fillet as it is. Nothing seems to work and my attempts so far have only produced strange looking corners.  I guess I need to do some more light reading…

In this example, surfaces tools are used to create the fancy candy bowl from the rendering. We begin by sketching the profile of the candy bowl on the Front plane and using Revolve to generate the solid.

Next, we need to make a few more sketches (all of them on the Front plane) that will be used to create surfaces. In the image, Sketch1 (in green) is the profile of the candy bowl that was used previously in the Revolve feature; Sketch2 (in blue) and Sketch3 (in orange) will be used to create the shapes of the cuts that will decorate the candy bowl. Notice how their endpoints are coincident.  Sketch4 (in red) follows the outside edge of the candy bowl (created by converting Sketch1 and then trimming to those two construction lines) and its endpoints are horizontal to those of Sketch2 and Sketch3. Sketch5 (in purple) will determine how deep into the thickness of the candy bowl the decorative cuts will go. Notice that the endpoints of Sketch5 are also coincident with the endpoints of Sketch4. One more thing to notice is that Sketch2, 3, 4 and 5 are one-curve profiles, with no segments. I used to have a couple of arcs instead, but I ran into trouble down the road while using some of the surfacing tools, so I used Fit Spline to join both segments together in one curve and it all worked out much better. It will all become clearer in a moment.

We’ll create an extruded surface using Sketch2. In the feature manager, pre select Sketch2 and from the Surfaces tab (or toolbar) select Extruded Surface.  A property manager displays, which is very similar to that of the Extrude feature.  We only need to extrude the surface far enough to intersect and completely go through the candy bowl, like in the image.

We do the same with Sketch3. The extruded surface created above is shown here in blue.

Now we are going to use Sketch4 and Sketch5 to create a couple of revolved surfaces.  First, pre-select Sketch4 and then, from the Surfaces tab (or toolbar) select Revolved Surface. A property manager, very similar to that for the Revolve feature shows up, as you can see in the image.  Note: the extruded surfaces we created previously are shown in this image in blue and orange. The preview of the revolved surface we are about to create is shown in pale yellow.

This image shows all the surfaces created so far: the two extruded surfaces appear in blue and orange, Revolved surface1, created using Sketch4 is shown in red, and, finally, Revolved surface2, created using Sketch5, is shown in purple. The solid body (the candy bowl) has been hidden, but all the sketches are still showing.

Now comes the really fun part. Using Trim Surface from the Surfaces tab (or toolbar), I’ll trim the two extruded surfaces, using the two revolved surfaces as trimming tools. I’ll start by trimming Surface Extrude2 using Surface Revolve1 as the trimming tool.  Notice the property manager in the image below.  A Standard Trim Type means simply that I’m using one surface as a tool to trim the other, as opposed to both surfaces trimming each other mutually at their intersection.  The trimming tool could’ve also been a sketch or a plane. Remove Selections means that the pieces of the extruded surfaces on the side I select (shown in purple right where the cursor is) will be discarded and only the pieces on the other side of the intersection (shown in pale orange) will be kept.  A Natural Surface Split Option means that the boundary edges of the extruded surface trimmed this way will be forced to follow the shape or the revolved surface used as trimming tool.

The same procedure is used to trim Surface Extrude1, using Surface Revolve2 as the trimming tool. The result of the trimming operations is shown here, where I’ve hidden Surface Revolve1, so you can notice the boundary edges of the extruded surfaces after the trim. Surface Extrude2 is shown in orange, Surface Revolve2 is shown in purple and the edge of Surface Extrude1 is that blue line on top of Surface Revolve2.  Notice the curvy edges of Surface Extrude2. They look that way because now that’s been trimmed, they follow the shape of Surface Revolve1 (the red colored surface not shown here).

Now I’m also going to hide Surface Revolve2, in order to have a better view of the two extruded surfaces we just trimmed. I’m going to use Boundary Surface to create a couple of surfaces between the boundary edges of the two trimmed surfaces.  It seems to me that this feature is, in a way, very similar to Loft, and, as such, it can become more or less complicated when more edges or curves are involved in the process. In my case, however, I only have a couple of edges, no guide curves and no curvature or draft applied.

The two resulting surfaces are now knit together into one using the Knit Surface command from the Surfaces tab (or toolbar). We need them as one single surface for the next step.

Next, I’m going to show Revolve1 (the candy bowl) again and cut it using Surface Knit1 as my tool. This is done by using the Cut with Surface command from the Surfaces tab (or toolbar).  This command allows you to cut a solid body or bodies using an intersecting surface. The direction of the arrow in the graphics area points to the part of the solid body that will be discarded.

After hiding all the surfaces, the result is a decorative cut that can be mirrored about the Right plane, and patterned to apply it to the rest of the candy bowl.

And voila! Nice, isn’t it? I think I’ll get that Surfacing book off the shelf and start learning about the proper ways to create this and other cool stuff using surfaces in SolidWorks!