Creo Explained – Part 5

<< Part 4

Towards the end of the previous part of this series I mentioned that I performed two operations to the block with the hole. I changed the radius of the round and moved the hole. I did that in two straight operations because I knew exactly what I wanted to do.

Let’s take this a little further. Say I want to try out stuff and am not entire sure of what I want to do. I know that I want to change the radius of the round, but I’m not sure exactly by how much. I increase the radius by 5 mm. Then increase it by another 2.5 mm. Next I realize that the correct increase should have been 4 mm and not 7.5 mm and so I decrease it by 3.5 mm. Say in all I change the radius five times. So after finally locking down the radius to the value I am happy with, let’s see what the model tree looks like when I open the part in Creo Parametric.

To my horror I see five new Edit Round features, one for each change in radius that I made in Creo Direct. Clearly this is not what I wanted to see. Ideally the round feature itself should have been edited with the final value for the radius. If you remember, Creo Direct didn’t do that earlier and instead added an Edit Round feature. Maybe I can live with that. But adding five new Edit Round features for what was actually a single edit round operation is nuts. Creo Direct isn’t smart enough to understand what I ended up doing. It blindly converts every push pull operation into some form of feature and slaps it to the end of the feature tree.

Just for fun I went back to Creo Direct and moved the hole around a few times. When I brought the part back into Creo Parametric this is what the model tree looked like.

This long feature tree may give  you the impression that the part is a complex one. But actually its just a couple of extrudes and a round, that’s all. Every thing else is me trashing around the model in Creo Direct, which ended up messing up the feature tree.

Now imagine if you created a complex part with a number of features in Creo Parametric. By features, I mean real ones like extrudes, rounds, fillets, etc. and not a bunch of edit and move features. Then say you give this file to someone who is using Creo Direct and the person pushes and pulls stuff to his heart’s content. Can you imagine what will happen to your feature tree? If the person is not an experienced user or is trying out stuff (which is quite a reasonable thing to do) it may turn out to be a bloody mess. The problem with Creo Direct is that since the feature tree is hidden there is  no way of seeing the kind of havoc the user is creating as he thrashes the model around.

Now coming back to my point earlier whether this implementation of Direct Modeling solves more problems than it creates, you tell me. In my opinion, converting each and every push-pull operation into a feature and bolting it to the bottom of the feature tree, especially without clubbing identical consecutive features into a single feature may not be the best way to do it. If you are someone who uses Creo Parametric and Creo Direct to model real world stuff I’d love to know what you think about this implementation of Direct Modeling. How does this “best of both worlds” solution work for you? Please do leave a comment.

Here is a nice video I found on YouTube that shows some nice round tripping of models between Creo Parametric and Creo Direct.

PTC is aiming Creo Direct at the “other people” in the enterprise. Folks like analysts who need to make quick design changes to validate their designs. For this kind of a direct modeling implementation to work properly the people using Creo Direct should be careful how they push and pull stuff around. Otherwise things may not look pretty when they hand back the model to the designers who created it.

Part 6 >>

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  • Jason Ma


    I wonder what happens when you edit the sketch in Creo Parametric to change the position of the hole (in the parametric way), does it invalidate all the move features down the tree, or does it add yet another one?

    • I just tried it. It doesn’t invalidate the move features below. It applies them one after the other. So now I have a situation wherein I moved the hole the “right” way (by editing the sketch) and when the model regenerates the hole does not sit where I asked it to. 😉

  • Jason Ma

    That’s interesting… 🙂 

    Thank you, Deelip.

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  • Geoff Hedges, PTC

    Hello Deelip,
    In Parts 4 an 5 of your Creo Explained blog, I believe your core question asks ‘Is the approach PTC’s taken with the AnyMode Modeling technology, Creo Parametric, Creo Direct and the Common Data Model, the best?’
    We believe so, and others seem to believe that too. It certainly follows the approach of ‘keeping it simple’, I’ve recapped the strategy, our approach, and also comment on other technology approaches on the following blog.

    Best Regards,
    Geoff Hedges
    PTC Marketing

  • aaa

    I have a different result after doing round change and moves.  Look like you did edit rounds and moves as completely different operations: Select geometry – pull, select same geometry – pull, etc.  Did you try to use undo to return to the last operation and change it?

    • Of course, undo will remove the last push/pull operation. But that’s not the point. Say if you are moving two faces of a box. You move one and then move the other. Then you move the first one back to its original position. That doesn’t remove the original move feature. It adds a third one.

      Creo Direct simply take every push pull operation and blindly creates a feature from it without bothering to look at the problem as a whole. I guess this could be done years ago. This is hardly breakthrough technology that PTC is making it out to be.

      • Oneil

        Assume that you move a face left and some element (like a hole) completely disappear as a result of this move. Now you move the same face right, the same distance. Do you want to see the hole again? If you choose “undo”, yes, you surely expects it. But if you consider the first move as some “final action” then you don’t have any memory and if the hole is gone it is gone forever, it can not be shown again.  So even in this simple example we see that  we can not  just add 2 opposite moves and consider that we do nothing, i.e. we can not just delete 2 move features in the history tree because it would lead to a different result (with the original hole).

        • nick

          Inventor Change Manager compares the effects of the two moves (in your example), and if they cancel out, nothing is added to the history tree. But if there is some difference (like some holes disappearing) then that difference is captured by a parametric history operation.

          • Precisely. This is the kind of intelligence that is missing in the current implemention of Creo Direct. I’m sure it will improve in time. But the point of this blog series was to explain how things are at present.