Alias Design For Inventor – Part 3

<< Part 2

Alias Design for Inventor merely adds “Alias Freeform” features to the Inventor feature tree. You can apply the free form feature to a single feature (eg. extrude) or an entire body (a bunch of features). Basically the free form editing happens by adding points to the edges of a model and moving them around freely in space (hence free form). The adjacent surfaces are adjusted accordingly. This is mainly used at the conceptual design stage when you are interested to quickly arrive at a basic shape which you can then refine later with dimensions, constraints, etc.

In a comment to Part 2 of this series Kevin Quigley wondered:

“One thing I’m not entirely clear about Alias for Inventor is how it slots into the history? Can you go back to the Alias feature and tweak the shape, or is it a one hit thing? How does the shape tweaking affect history if you make changes that add faces or remove faces, so the “tag” to the faces changes?”

Yes, theoretically you can go back and edit the free form feature anytime you want. You can add new points to the edge curves or move/delete existing ones. However, in practice, depending on where you insert the free form feature in the feature tree, the results may or may not be as per your expectations. This is a little complicated and cannot be explained in words alone. So I am going to do this by means of a simple example.

Consider a simple model with two extrude features, one depending on the other.

Lets say I created the big box first and then the small box using one of the faces of the big box. Let see what happens if I apply a free form feature to the face holding the small box.

As you can see the small box rebuilds fine and there are actually two disconnected solid bodies, although Inventor still reports just one. Not sure why.

I added the free form feature to the big box and not to the entire model. That’s why the feature appears after Extrusion1 and not at the end of the feature tree. Now lets add a free form feature to the smaller box.

As expected the feature tree now shows a second free form feature after Extrusion2.

So far so good. Now say I want to edit the free form feature on the big box. I add two new points to the curve to give it a better shape.

Note that when editing the free form feature on the big box, the small box disappears. This is because at this point in the history of the model the small box does not exist. So after I edit the free form feature on the big box I expect Inventor to rebuild the model and show me the change that I made. Instead I am surprised to see the old shape. Hovering over the first free form feature in the feature tree shows me this.

The highlight tells me that Inventor has recorded my change to the first free form feature. But somehow it is not being reflected in the resulting geometry. Interestingly hovering over the second free form feature shows me this.

The highlight signified that the second form feature includes the first box and its original free form feature as defined when the second free form feature was created. So this means that cascading free form features kind of lock the geometry preceding them. To confirm this I carried on with this experiment by adding a third extrude feature and applied a third free form feature to it. I then went ahead and changed the first and second free form features and they didn’t get updated in the geometry. However, hovering above them in the feature tree did indicate the changed definitions. If I suppressed or deleted the third free form feature my change the the second free form feature was shown, but not my change to the first free form feature. If I suppressed or deleted the second free form feature then the changes to the first free form feature were shown. This proves that when you insert a free form feature the geometry preceding it is locked down. So much so that if I edit the sketch to change the dimensions of the big box, the geometry will not update to show the changed size.

From this little experiment one can conclude that having free form features depending upon other free form features is probably not a good idea if you want to come back and edit them, which you most probably will want to. Instead it is much better to add a free form feature at the end of the feature tree or at the end of the set of connected features which form a particular part of a model that you will want to modify as a whole later on.

I rolled back to the original two box model and added a single free form feature to the entire body. I then tweaked the edge of the big and small box in the same free form operation to get this.

Later I went back to the free form feature and tweaked the edge again and got this.

So now I have total control over all the edges of this model (or this part of the model to be precise) because they are all in the same free form feature.

The above answers only one of Kevin’s questions. He also asked what would happen of you added or removed geometry that a free form feature depends on. I haven’t even reached there yet. That is the subject of the next part of this series.

Part 4 >>

  • Nainar

    The feature tree from the outside may look like a tree but internally in most of the software it will be a graph. And there is potential risk of introducing instability by doing the way you did, creating something called cyclic dependency, which is why one of them is locked to prevent infinite cycling of the graph.

  • http://www.deelip.com Deelip Menezes

    Actually, I never liked the term “tree”. A tree implies many branches and different paths. The feature tree is just a list of features, that’s all.

  • Nainar

    To go to a leaf in a tree, there is always a single path, even if there are multiple branches right? That is what matters in parsing the tree. One needs to have a unique path to have the same solid everytime it is rebuilt.There are many many interesting scenarios if you try Assembly level features with UGS and Parasolid( Can’t think of any one else providing that fantastic feature ).Like one leaf on one solid referring to another branch in another tree!! Wonderful complication for a designer to play with when doing top down design.

  • http://www.deelip.com Deelip Menezes

    I think the term “tree” came about because of the GUI tree control that was used to represent it.

  • lzprgmr

    >>As you can see the small box rebuilds fine and there are actually two disconnected solid bodies, although Inventor still reports just one. Not sure why

    I guess Inventor will only created a new solid body only if you asked it to (there is an option when create feature), or else it will always stick to one body, but multiple lumps… as this is how inventor behaves before the support of multi-body




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