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Monthly Archives: September 2011
September 28, 2011Posted by on
You can create sketch implicitly while creating the swept surface.
As stated above, instead of explicitly creating a profile sketch, you can sketch it while creating the swept, which, in fact, is recommended as well.
Let’s see how…
Consider the following example, in which the guide curves are drawn, with reference surface, and the profile sketch needs to be created. So select the adaptive sweep tool, select the guide curve (yellow colored).
Now go to sketch selection and select the sketch tool placed besides the selection box. The software prompts you to select a point, so select one (blue colored). The point can be any geometric point, explicitly created or even a vertex of the guide.
Note that the current model contains three guide curves (red, white and yellow). You can select as many guide curves as required.
Now select the remaining guide curves (white and red) one by one and hit OK. You can select aggregated sketch and positioned sketch to create them so. (aggregated means the sketch will be there beneath the adaptive sweep feature in spec. tree, and I guess you already know what positioned sketch is).
The software automatically finds and creates intersections of the selected guide curve with the sketch plane (which will pass from the selected point – blue one). Create a desired sketch now and exit the sketcher. Select spine if required and hit preview and OK if the result is as required. Here’s in our case…
Thanks for reading! Keep visiting for more…
September 25, 2011Posted by on
A swept surface which maintains constraints assigned for the profile sketch with guide curve.
As stated above, adaptive swept surface is a little different than those created using the sweep tool. In distinction, it can be stated that the adaptive swept surface retains the constrains – dimensional or geometric – created for the profile sketch with guide curves. A good example will be required here, so let’s have one.
The tool we are talking about is a Generative Shape Design (GSD) command, so start the workbench from the Start menu > Shape > Generative Shape Design. Or even you can create a new CATIA part and then switch between workbenches. Let’s first create a surface with the standard sweep tool. First create the sketches for a profile and two guide curves (we’re gonna use explicit sweep with two guide cures subtype). Figures below state the rest. Images are for illustration only and, obviously, you can create your own sketches instead on those shown here.
Profile sketch…..(YZ plane)
Guide curve 1 sketch…..(XY plane)
Guide curve 2 sketch…..(XY plane – can be any other plane as well)
Make sure that the profile is intersecting with the guide curves, otherwise you have to define the intersection manually while creating the swept surface as anchor points. As you can see in the above sketches, several constraints have been applied for the profile sketch and or the guide curves as well. Now let’s create the swept surface. Select the Sweep surface tool from the surfaces toolbar.(or go to Insert>Surfaces>Sweep…) Image below shows the sketches with graphic properties applied for better visualization.
In the swept surface dialog box, select the explicit as profile type and With two guide curves as the subtype. Select the profile, guide curve 1 and guide curve 2 in their respective boxes. Clicking on preview results in the swept surface as shown. (the second image shown result if you alter the guide selection)
As one can see, the surface being created in both the cases, the profile have been modified to adjust with the guide curves. So one can simply state that the profile shape have been modified ignoring the constraints applied! The result is quite acceptable if you really wanted so. But suppose I want to maintain the constraints applied in profile sketch throughout the surface (say arc radius in our case), then? That’s why I’m writing this post!! Adaptive swept surface is the tool which will do this for me.
Now, before we switch the tool, there are certain things need to be taken care of. It’s advisable to create the profile after creating the guide curves as you’ll be assigning constraints for the profile end points to be coincide with the guides. For this you can find intersection of guide curves with the profile sketch plane and assign the remaining constraint. Also the profile sketch requires to be under-constrained, meaning to say, you can assign as many constraints as you want in the profile, until there are enough entities left to adjust with the guide curves. In our scenario, I’ve assigned the arc radius and center point height from the horizontal axis. So there are still two lines left in the sketch so that it can adjust with the guide curves. Concluding, assign constraints for only those entities which required to be same in shape and size. So I hope you’re well capable to do that.
Do as said above, and select the Adaptive sweep tool from the surfaces tool bar or from the pull down menu bar. Select the guide curve first from the two we’ve drawn earlier(it’ll be the default spine as well), and select the profile sketch(a warning may appear if the sketch contains irrelevant, or rather, unsolvable constraints). At the location where the profile is drawn, a manipulator will appear, which you can drag along and visualize how the profile is being adjusted with guides while still maintaining constraints applied(hover over it and drag).
Click preview to see the surface and hit OK if the result is as required. We’re done here! You can measure radius of the curve at the other end to verify it’s the same as you’ve created.
Now, let’s consider another scenario, shall we?
As as a guiding curve, you can select sketches, 3d curves, or even surface edges as well. Even you can assign constraints of the profile sketch with any 3d face as well. Keep one thing in mind however, if the guide curve or the surface is a multi-cell element, you need to create a Join feature first and then use them, otherwise error would not be far away. Let’s consider the case with 3d curve as shown in the image below. The 3d cure is created with Combine tool, which is in fact a multi-cell element. So while creating the profile sketch (coffee colored), I’ve used combine feature (again combine feature) to find intersection with the sketch plane. Instead, if you select an element of combine, it’ll find intersection for the entity selected only, not for the whole combine curve. So beware, otherwise error will be prompted.
Now select the yellow curve as guide curve, select the profile, and hit preview. Click OK if everything is fine. The surface is shown here.
So let’s finish up the design end see what we end up making by creating additional features.
Let’s now apply materials and create a rendering so it looks realistic.
This is what we finally got!
Thanks for reading the post. Comments and suggestions are welcomed! Keep visiting for more.