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Ever had a sweep that just seemed to give errors and did not want to form the way it should. One thing we at CDC have learnt is that CATIA has almost no limits as to what can be done with Surfacing. There is always a way! This CATIA tutorial will show you how to control a sweep more effectively.

Here we have an extruded surface created from a door punch surface. Now we would like to pinch a new surface inward at 45deg to the extruded surface and at a length of 70mm.

Here everything looks fine but if we increase the sweep length to 250mm, we can see that the surfaces are 45deg but the direction is wrong and there are warnings that appear (still nice that CATIA can generate a surface though (“,) ). This is because the 45deg is normal to the surface, so in sharp corners errors will normally occur.

So, how do fix this sweep? Easy… we give it a back bone or a “spine” to give it some sort of direction. We create a sketch an in it a circle. The dimensions of the circle are not critical.

Now back in the Sweep definition, we need to add the sketch as a spine. And then on preview we can see how smooth the sweep is now.

Set the sweep length back to 70mm and know that it is much easier to manufacture now as the surface is smooth and has no sharp edges or undercuts.

I hope you enjoyed this CATIA Tutorial brought to you compliments of CDC your technology partner.

This CATIA tutorial shows you how to Create Scenes and use them for Draughting

Ever created an isometric view in the Draughting work bench of an assembly, then changed the location of parts in an assembly and when you go back to your drawing you find it has updated the drawing to that of the assembly. This is good to have as it is part of the power of CATIA with its associativity. But sometimes you want views to keep their positions, i.e. you want an assembled isometric view as well as an exploded view.

We have our assembly…

We create an isometric view…

Now the problem arises when you edit the main assembly and then the drawing up dates as well. So we need to create a scene, for exploded views or even where only specific parts are shown.

Make sure you select the full overload option before clicking OK.

Hide, show, move and rotate parts until you get the view you want and then click to exit the scene (same icon as exit sketcher), you can see in the tree that there is a new Scene.1 that has been created.

Here are only a few parts that need to be shown…

An exploded view…

Now to apply these scenes to the drawing, double click on the scene you want, then from the Draughting workbench create a view and in your assembly which should be in the scene you want click on the Scene you want in the tree first, then click on the model to generate the view.

In CATIA you can create your own Power Copy’s.

These can be fairly intricate operations…

Follow these steps to create a simple power copy and try to expand on this yourself adding more features as you go…

• Start with a new part and a pad
• Create a 3D point on one of the faces
• Create a sketch on that same face and create a circle that’s centre is constrained to the 3D point created. Add a diameter dimension to the circle
• Exit Sketcher
• Create a simple pocket
• On the bottom edge of the pocket create a chamfer

Now say you have to create lots of these… you don’t want to have to go through the same process over and over again… This is where we will use the Power Copy to speed things up a little.

• Go to Insert > Knowledge Templates > Power Copy…
• Now you need to select what you want to include in your Power Copy
• Select the Pocket.1, Sketch.2(sketch for the pocket) and the Chamfer.1
• You will see on the right, in order to create the Power Copy you will need a pad face and a 3D point
• Click OK

• Create another 3D point on a face where you want to create this pocket and chamfer again
• Click Insert > Instantiate from selection
• You now need to make two selections the face and the newly created point
• Click OK and see your power copy

• You can do this a few times

Generaly CATIA can open large assemblies without a problem. But sometimes the assemblies get really big… waht makes CATIA so powerful is the fact that you dont need gorilla machines to open large assemblies, just a quick change of settings and off you go.

• Go to Tools > Options > Infrastructure > Product Structure.

• Click on the “Work with the cache system” check box.
• You will get a message that basically tells you that you need to restart CATIA for this setting to be applied.
• Click OK but don’t close CATIA.

• Go to the Cgr Management tab.
• Click in the “Optimise cgr for large assembly visualisation” check box.

• Click OK and then close CATIA.
• Reopen CATIA.
• Open the model that you are having trouble with.
• In the screenshot below I opened an entire Chrysler assembly in about 30 seconds on a laptop (the cgr files had already been generated – if they had not, it takes about 4 minutes to generate and 30 seconds to open)

• It has basically loaded lightweight cgr files.
• If you want to work on a specific part or assembly just double click on it can CATIA will load the actual part for editing.