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Archive for the ‘Assembly 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.

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.

This blog post was inspired by a question I received via email. The question was about how to create a section view in an assembly.  There was a picture attached to the email that showed an assembly  that seemed to have been cut along two planes, but only partially, and  it appeared that one chunk  of the assembly had been removed to reveal the inside, while the rest of the assembly remained visible, similar to cutting a slice of a pie.  I was in a bit of a hurry, so I tried to explain myself really quickly, but then I thought that it was actually a very good question, and it may help a few other readers out there if I answer it here, as well.

For illustration purposes, I’m going to use this old model of a drill jig. Suppose I want to create a section view of this assembly by making a partial cut along the Front and Right planes and removing a section of the drill jig’s handle and  block, thus revealing the screw inside.  If I tried to use Section View  (from the Heads Up Toolbar in the Graphics Area or  from View, Display, Section View), it would slice all components in the assembly all along  a couple of planes parallel to the Front and Right planes, leaving just a piece of it, as you can see in the following image. That’s not really what the section view of the assembly in that picture was supposed to look like.

So, let’s try a different approach using Assembly Features.  First of all, I created a new configuration and called it Section View.  Now, on the assembly’s Top plane, I sketched a couple of lines right where I needed the cut for the section, as you can see in this image. Notice that this sketch in on the assembly’s Top plane, not at the part level.

Once my sketch was ready, I clicked on Assembly Features from the Assembly toolbar and selected Extruded Cut from the list to cut the components in the assembly using my sketch (you can also find this command from Insert, Assembly Feature, Cut, Extruded Cut).

Notice that this extrude cut command works pretty much in the same way it does for parts, but rest assure that the components themselves won’t be affected by this feature outside of the assembly. As a start condition, I decided to use offset, so the cut would begin a short distance from underneath the sketch plane. Under Direction 1, I reversed the direction to extrude trough all in the upward direction.  This way it won’t cut all through the bottom of the block, but only through the top. I used Feature Scope at the bottom of the Property Manager to select that only the handle and the block, but not the screw, would be affected by the cut. You can see all my selections in the following image.

Here in this other image you can see the section view that was created this way. In the Feature Manager, a new cut extrude feature has been added at the assembly level. This feature only exists inside the assembly; if you open your parts in a separate window, they’ll remain unchanged.

I’ve never really been a car enthusiast. I mean, I like race cars and I sure enjoy the looks of a few models, like this particular one that was parked at some sort of car expo near the amusement park a few weeks ago. Isn’t it a real beauty? I actually like this one better than its younger cousins that were also on display that day.

 Anyway, I like to look at cars and I like to drive them, but I’m certainly not the kind that can remember makes and models, let alone identify all the different pieces that form part of a vehicle.  Last night, however, and out of sheer curiosity after reading a post from the SolidWorks Discussion Forums where someone was asking for examples on how to use the universal joint mate and someone else suggested looking at a drive shaft, I found myself searching the internet, trying to find pictures and information about cars and transmissions and what not. I eventually found some really nice assembly pictures for a 280Z, and my husband,  who  by then had grown curious about my sudden interest for cars, was more than glad to explain to me how each of those parts was supposed to work.   I never thought I would say this, but it was actually very interesting and even kind of fun.  Or maybe he’s just a good teacher, who knows?

This is one of the images I found for the drive shaft.

After taking a long look at it, I went back to SolidWorks to try to find some information on how to use the universal joint mate, but I couldn’t find much in the help. I guess it’s because it’s not really such a complicated mate?  So, I put together my own universal joint assembly to experiment.  The universal joint, also known as Hooke’s coupling, is used to connect two intersecting shafts, and apparently has its widest use in the automotive industry.  A simple model of the Hooke-type universal joint is shown in the following image. The small shaft could be the driver, the long one could be the follower and the third link is a cross piece that connects the two yokes. 

 As the driver rotates, it transfers this rotation to the second shaft.  In SolidWorks, the universal joint mate is useful for those cases when you need to transfer rotational motion around corners or, like in the case of the driver shaft of a car, between two connected shafts that are allowed to bend at the connection point.  

I actually came up with two versions of the same assembly, one with the third link connecting the two shafts, and one where that link is missing. The one without the link uses the universal joint mate, while the other one relies on the link to transfer rotation between the shafts. The results of using one method or the other were pretty much the same.

So, to add a universal joint mate between two components, simply  select  it from the mechanical mates group, and then, under Mate Selections,  select the two components you wish to mate together (in my case the two yokes)  and, as an option, define the joint point.  The joint point (in purple in the image) represents the connection point between the two components. In this case is the point where the axis of one shaft intersects the axis of the other.  Since I didn’t have a physical component connecting both shafts, I actually sketched a point to serve as joint point and located it where the center of the missing link would be.  Just as in the case of other mechanical mates, such as gear mate and rack and pinion mate, this mate will work even when the components don’t actually touch each other or have any other component to come in touch with both and connect them, but you’ll need to add other mates to the mix in order to control the position of the elements in the screen and with respect to each other. In my case I mated the axis of each shaft coincident with a couple of reference axes that intersect each other at the joint point.

I added a rotary motor to the driver shaft and then ran the motion study.  I’m sorry I didn’t actually make a video of this one, but it’s only ten seconds worth of animation, so I didn’t see the reason for it. This is an animated gif; if you double click on it you’ll be able to see the movement of the universal joint.