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Using the Combine Feature in Part Design

Using the Combine Feature in Part Design

Using the Combine Feature in Part Design

In the CATIA V5 Part Design Workbench, there is a small toolbar called "Advanced Extruded Features" with two tools on it by default.  One is the stiffener tool and the other is labeled "Solid Combine".  My experiments with the Solid Combine tool have only produced confusing results so far.  Does anyone know how to use it?

I don't have access to the online docs either.  If anyone knows a way to get remote access to those that would be helpful too.

Thanks in advance,


RE: Using the Combine Feature in Part Design

Combine works with two profiles (two sketches) to create a solid.

Pretend you're a draftperson. Make one sketch look like a front view, and the other sketch look like a side view, with the sketch planes perpendicular to each other. The two views (sketches) should align with each other. Now, use the COMBINE tool to combine both sketches to create a solid.

The examples in the on-line help files are not that clear.

RE: Using the Combine Feature in Part Design

Thank you for the reply Jackk.  The tool sounds interesting, but somehow not very valuable after the acceptance of parametric design concepts.

What I am hoping for is a tool that will morph a circular profile into a co-linear rectangular profile.  In the past I have abutted circular and rectangular pads together and argued with the fillet tool until the part resembled my intentions.  I am hoping for a more elegant approach.  Do you have a suggestion perhaps?

Best Regards,


RE: Using the Combine Feature in Part Design

Well, actually combine is extremely useful when you need to make center curves, spines, or other supporting geometry for surfaces.

I think that this is what you want to do....  

NOTE:  DO NOT use the "datum" option.  We want everything to maintain history, per this example.


With both of your profiles displayed, insert some combine points, by intersecting the circular profile, at whatever points you wish to terminate the blend vertex.  I chose to intesect the planes inside the circle sketch, and then do point intersect.  this will keep everything updated, if you change the value.


Make a plane, using one point and one line.  Use the vertex point, and the lines of the rectangle.


Make another sketch on the same plane as the circle sketch.  It will be a rectangle, and although you shouldn't normally do this, CONSTRAIN the rectangle to be tangent on all sides to the circle sketch.


Using the planes just created, make sketches outlining boundaries for a a "square to square" transition.  I have chosen to do 1/4 of the part at a time, so that I can simply apply a transformation.  Go ahead and put in the surface, and use the "join" command between them.

NOTE: I forgot earlier, but you will need to extend edges (that go throug the vertex) just a bit, because you cannot create a radius to a zero value, such as a point - as would be the case if we did this - see next picture)


Use the "variable fillet" tool. Set the radius near the circle to the value of the circle radius.  Set the radius near the rectangle to a NON-ZERO value, even if it's infintessimal.  Hit the "more" button (still in variable fillet) and check the box next to "circle fillet."  Use a spine created from the sketch planes for the circle and rectangle.  Hit enter.

You can trim and transform.

If you are proficient with knowledgeware, you can tie the first radius value to the circle radius, so that you get instant updates.  Even better, you can put all of the values in a design table, and make the value for the big fillet radius equal to the value specified for the circle radius. (using a simple excel formula)

Hope all of this helps.

RE: Using the Combine Feature in Part Design

There is a much easier way of doing that, however.  Use the GSD Multi-Section Solids tool.  It's also available in GSD as the Multi-Section Surfaces.

RE: Using the Combine Feature in Part Design

^^ Yah. I've never really found a compelling reason to use Solid Combine.

RE: Using the Combine Feature in Part Design


catiajim (Aerospace)      
16 Jun 05 9:11

There is a much easier way of doing that, however.  Use the GSD Multi-Section Solids tool.  It's also available in GSD as the Multi-Section Surfaces.

It's not easier at all, actually.  You have to create the initial geometry, anyway.  You have to know how the geometry will flow, beforehand.  Either method requires the same elements.  Either method, at least by my calculations, requires the same amount of steps.  Actually, the "multi-sections," formerly known as "loft," also requires trimming, which is built into the variable fillet.  Additionally, from a design standpoint, the variable fillet parameter is more visible, and easier to understand.

I will NOT dispute that your method is valid.  And, we all know that there are many ways to do the same thing.  Please don't take it as that.  I just don't agree with the part about it being easier.  Going through the example step by step with both methods will prove that EITHER one is not necessarily any easier than the other, although I do believe that the variable fillet method will save steps.

RE: Using the Combine Feature in Part Design

I just briefly looked through this thread and I do not really understan what a solid combine or even a curve combine has to do with filleting or multi-section surface.
I have used the curve combine function when working with A-class surfacing because it's a lot easier to smooth curves in 2-d than 3-d so smoothing the curve in to different planes and then combine them is very useful.
When I started with V5 I also bumped into the Solid combine function just because I'm a curious person and I thought it was brilliant!! Using two sketches in perpendicular planes to create one shape and of course if both those sketches are parametric as well whaoo!! so easy to change even if you just create a simple bracket and one sketch defines the thickness in sideview and the other sketch defines the shape in top view and whoola! you have a bracket that you can easily change your thickness and of course the shape by changing the sketches.
It's a good tool that most users will not use because they are not willing to experiment with new tools.
Perhaps we should all go back to the Drawing board why change something that works?

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