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Archive for the ‘Part Modeling’ Category

Hey there!   How is your Summer? Mine, so far, is just as I expected: hot and hectic. But I won’t complain. Instead, I’ve prepared a document with step-by-step instructions on how to make this pair of scissors that were used for one of the examples in my Easy Surfacing Techniques presentation.

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)

Hey there,

It took me a bit longer than I thought, but here it is: the tutorial for the hairbrush in pdf and the pack an go of the assembly. The model was saved in SolidWorks 2010, but the steps in the tutorial are good for previous versions too. Hope you guys find it useful!  You can download the files following the links:

Hairbrush tutorial on pdf

Hairbrush assembly pack and go

I’ll also add these links to the list of Downloads.

I hope you are not growing tired of my SolidWorks World chronicles just yet, because I still have a lot more to write about. This was a particularly good SolidWorks World for me and I want to share what I learned with you.  This time, let me tell you about yet another hands-on session I attended. This one was presented by Michael LaFleche, Regional Technical Manager for CAPINC, and it was an introduction to direct modeling techniques in SolidWorks for those of us that hadn’t really tried that functionality before or didn’t know how we could benefit from it.

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.

This one was the first ever hands-on session I attended at SolidWorks World. Last year I wasn’t able to get into any of the hands-on sessions, but this year I had the opportunity to pre-register for several of them and it was one of the best things I could’ve ever done. 

This session was presented by Dan Riffell, Projects Coordinator at Eltron Research and Development. Dan is also a very well known contributor in the SolidWorks discussion forums and engineering community. Dan prepared this session because, believe it or not, how to model a thread is an incredibly common question among SolidWorks users, so he wanted to explain a few different ways to do it that may be useful depending on our needs.

First of all, Dan began by pointing out that we usually don’t need to model threads. Unless we need them for an animation, mold creation or a photorealistic image, for instance, most of the time, we can get by with using annotations and don’t really need a physical representation of the thread in the model. We can add a callout in the drawing with information about the thread or use a special kind of annotation known as cosmetic threads (Insert/Annotations/Cosmetic Threads).  

This kind of annotation appears as a feature in the Feature Manager and you can suppress it or delete it if you don’t need it anymore.

He then showed us how to create revolved threads. He sketched a thread profile and revolved it around the temporary axis of the part, creating a cut ( Revolved Cut), then he created a linear pattern using the revolved cut as the feature to pattern and the part’s temporary axis to define the direction.

Notice that this is not a real thread, but only looks like one, and it’s actually the kind of thread that is usually generated for most Toolbox screws.

The next method that Dan demonstrated involved the use of Swept Cut, as you can see in the image. He used the same thread profile sketch as before as the profile for the cut, but this time we had to create an extra sketch to be used as a path. It was a simple sketch of a line that runs along the axis of the part. The option to twist along path is what makes the profile describe a helix as it travels along the path.

The next method is very similar, but he creates a helical surface first and converts its edge into a 3D sketch to use it as a path for the Swept Cut command. This is similar to what Charles Culp did to create the telephone cord, remember? Notice that this time around the path is already describing a helix, so there’s no need to use the option to twist along path.

Another method to create a helical path for the thread is to simply create a helix by using Insert, Curve, Helix/Spiral, as you can see in the following image. By the way, to use this method you have to start by opening a new sketch on the circular face of the part and converting the edge to use it as the base for the helix. A curious fact: I asked Dan if it made any difference what start angle we chose and he said the rebuild time changes with the angle, for some strange reason.

Once you have the helix ready, you can use it as the path for the Swept Cut, and, just as before, there’s no need for the option to twist along the path.

 

What Dan demonstrated next was the coolest part, because he showed us how to create a design library feature to add threads to other similar parts without having to go through the whole process again and again.  First, he opened the Design Library Tab in the Task Pane and dragged the SweptCut1 feature from the Feature Manager tree  to the Design Library’s lower pane. A property manager appeared, as you can see in the image. From this property manager we can choose a folder where to store our new library feature and/or add a tooltip to remind us what this library feature is for.

Once the library feature has been added to the design library, we’ll see it in the lower pane or in whatever folder we placed it and we’ll be able to use it in other parts simply by dragging it from the lower pane and dropping it on the graphics area. In this example, after we drop the library feature, SolidWorks prompts for us to select a placement plane. Other selections will be necessary, as well (an edge, a sketch point and a face). All these reference selections are defined by the relationships that were used in the thread profile sketch. For instance, the thread profile was sketched on the Front Plane, so the Front plane should  be our selection for Placement Plane.  A little display pops up to help us along the proces,s by giving us visual clues of what we’re expected to select. In the image below, for instance, we are expected to select that circular edge we see there.

Once all our references have been selected, the thread is added to the part.

Last but definitely not least, Dan showed us how to model an inner thread, such as the ones in nuts, to match the outer one. We started with the model of a nut and inserted the screw we had been working with before by using Insert, Part.  We located the part as you see it in the image by adding a concentric mate  and a distance mate between both parts.  Remember, this is not an assembly, we inserted a part into a part.

Next, Dan showed us how to use Combine (Insert, Features, Combine) to subtract the screw from the nut, as you can see in the image. The nut is the main body (in green) and the screw is the body to subtract (in blue).

As a result of this operation, SolidWorks will remove or cut away the parts of the nut that overlap the screw, creating the inner thread. Neat!

As I said before, the step by step procedures and files for this and other presentations will be available in March. For now, I hope my little summary may be helpful to somebody.

Thank you, Dan, for this great presentation!

Part of the freedom I’m longing to experience this year is simply putting the fun back in what I do. Not everything needs to be solemn and extremely important, at least not all the time. So, with that in mind, I was working on this model of a hairbrush, just for the sake of practicing and having fun. I must admit, given the kind of item it is, I also thought it could provide a few examples on using patterns. I have a few patterns in there, as you will see in just a few moments. Some of them are feature patterns and there are also a couple of  component patterns, as well. I had a particular brush in mind, so I tried to make it look exactly like the real one.

First, I started with a simple extrusion. I sketched an ellipse on the Front plane, centered on the origin to take advantage of symmetry, and extruded it to create the part of the brush where the bristles will be. I made a couple of extruded cuts on both ends, using arcs that were sketched on the Top plane. In this image you can see the sketches in pink.

 

After that, I sketched a circle on a plane parallel to the Front plane and used it to create a loft between it and one of the edges of the elliptical extrusion, as you can see in the following image. I used the start constraint normal to profile (start profile is the circle) to shape the loft a bit and make it look more like the brush I own.

 

After the loft, I shelled the whole thing to a thickness of 0.18 in, because my real hairbrush is hollow.  Notice that I didn’t remove the circular face on the other side, but only the one highlighted in blue in the image.

Next step was to create the zigzag cuts on the hairbrush. For that purpose, I sketched a zigzag line on the Top plane, symmetrical with respect to the Right plane, and used Offset (look for it in the Sketch tab) to transform it into a slot with circular capped ends, as you can see in the following image.

I used the sketch of the slot to extrude a cut through all in both directions (up and down) and then, after filleting the edges a bit, I used Linear Pattern to reproduce the cut and the fillet features nine times along the body of the hairbrush, as you can see in the image. I used the line of symmetry in the sketch to specify the direction of the pattern.

Trying to make holes for the bristles was the fun part. In the real hairbrush, there are nine holes per row (except at the top where there’s only seven) and they are all located along a zigzag line that follows the same shape of the slots used for the cuts. At first, I thought about simply sketching a zigzag line or offsetting the previous one on the Top plane, drawing some circles along that line (still on the Top plane), and using them to extrude cuts for the bristles. However, this approach would not work fine, because I overlooked the fact that these holes would be created with projections of the circular sketches and would therefore deform and/or show in a position different to the one I expected.  So, what I ended up doing was to offset the first zigzag line (the one for the slot) and then project it on the face of the hairbrush, to have as my guide for the holes.

I also created a couple of reference points on the face of the hairbrush and right in the middle of two of the line segments, such as the one you see in this image.

Using those two points and the points at the end of each line segment, I created a series of planes that were tangent to the face of the hairbrush and that passed through each those points.  One plane per point.  On each plane, I sketched a circle and used it to make a hole for the bristle on that location, as you can see in this image.  These holes are not deformed like previously.  I only had to cut half of the holes in the row and then mirrored with respect to the Right plane to create the other half.

Once I had all the holes in place in that first row, I used a Linear Pattern again to recreate the holes nine times along the body of the hairbrush in one direction. Again, the direction for the pattern is specified by the same line in the slot sketch that I used before.

I used Linear Pattern one more time to recreate a row of holes in the opposite direction, only this time, as you can see in the image, I left out the hole on the edge, because that one doesn’t fit on this row. This step only created half the row, so I had to mirror the other half with respect to the Right plane.

After adding a few fillets to the brush, just to make it look a little nicer, I continued with the handle by creating a second loft, this time between the circular edge of the brush and an ellipse sketched on a plane parallel to the Front plane, as you see in this image. I used start and end constraints to shape the loft a bit. By the way, the start constraint “Normal to Profile” simply means that, on that side of the loft, if your surface was a mesh of parallel lines going from one profile to the other, the lines would try to remain normal to the elliptical profile, at least for a while, depending on the start tangent length.  On the other side of the loft, the end constraint “Curvature to Face” means that the surface of the loft is trying to follow the same curvature of the face of the brush that is highlighted in blue, at least for a while, also, depending on the end tangent length.

OK, so, let’s continue with the handle. Next, I offset the elliptical edge a bit and created an extruded boss for the handle. I also added a Dome feature at the end. On another plane parallel to the Front plane, I created to ellipses by using Convert Entities on the edges of the handle and the second loft. I used this sketch to extrude a cut on the handle, as you can see on the image.

Once again, I used a linear pattern to recreate this cut thirty times along the handle, in order to create the ridges I saw on the handle of the real brush.  Next, I cut a circular hole on the part of the handle without any ridges on it. I guess some people may use this hole to hang the brush from a hook. Personally, I keep mines inside a drawer. Anyway…  I sketched a couple of circles on the Top plane and used them to extrude a little edge around the hole, as you see in the following image. Notice the end condition on both side is “Offset to Surface”, where the surface is the one in pink, this way the extrusion follows the shape of the handle.  I had to select the options “translate surface” and “reverse offset” in order to make it work.

The last step was to create a bit of a “ridge empty” surface on the handle, for the brand or tag. I did this by sketching a slot on the Top plane and extruding it, just as before, using Offset to Surface as the end condition. Only this time I didn’t select translate surface, however, as that would’ve resulted in my new surface having ridges just like the rest of the handle. 

The bristles were created separately. Well, I must actually say “bristle”, singular, because I only created one and inserted nine instances of it to an assembly I created from the hairbrush body part. I mated all nine bristles on their correct holes in one of the rows and then used a Feature Driven Component Pattern to reproduce bristles in their correct holes in all other rows, as you can see in the image. This is only in one direction, because my driving feature is the Linear Pattern I used previously to create holes in these rows, remember? I guess I could’ve done something similar by simply using a Linear Component Pattern instead, but by doing that I would’ve had to enter the correct distance to the holes, etc. This way, this pattern will be linked to the other one and if that one changes, this one will update with the right information.

I did the same on the other direction, to create the last row of bristles, only I didn’t pattern the bristles on the edge, since there’s no room for them on that row. And that’s it! I hope you found this useful, or at least fun.

 

 

This is how the brush looks like finished, without appearances.