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rpostak1-Visitor
1-Visitor
September 14, 2015
Question

Advanced Surfacing Techniques

  • September 14, 2015
  • 6 replies
  • 13441 views

Hello to all,

I am new to the PTC CREO world, but I have over 30 years of CAD experience in other softwares and 20 of those 30 years have been all parametric modeling.  I am currently using CATIA V5 here at work and I am in the process of evaluating CREO for our engineering department.

So my question is...after importing a surface from CATIA into CREO, where do I go and/or how do I extract the edges of the surface as "curves"?

6 replies

D
DeanLong1-Visitor
1-Visitor
September 15, 2015

Set the selection filter (Lower Right of the screen) to the Geometry.

Select the "edges" you want (hold control if you want multiple)...CNTL C, CNTL V and it will copy them. You can use the tool bar Copy, Paste as well if you prefer that better.

    D
    DeanLong1-Visitor
    1-Visitor
    September 15, 2015

    Richard,

    A second thought crossed my mind in regard to your question. You state you are evaluating Creo but asked how to copy curves in reference to surfacing. Are you looking at converting V5 surfaces to Creo with the same fidelity as the native by copying imported curves? Are you importing simple stuff (ruled, revolved, lofts, blends) or are you copying more complex stuff?

    I ask because, while somewhat similar, V5 and Creo have difference methodologies when it comes to some of the deeper stuff.

    R
    rpostak1-VisitorAuthor
    1-Visitor
    September 15, 2015

    Dean,

    Typically when designing a window for a customer my starting point is their referenced OML (outer mold line) surface which is basically the outside surface of the aircraft and a set of curves wihich defines the window opening.  From that point I start offsetting the curves along the surface to use as construction geometry for splitting the surface ( a V5 command).  This is my methodology in CATIA and also how I would like to generate the same data in CREO.  Now this could be considered an advanced surfacing technique in CREO, but any help would be greatly appreciated.  The customer's surfaces could be simple or complex depending upon the shape of the aircraft's cockpit.

    C
    Constantin15-Moonstone
    15-Moonstone
    September 15, 2015

    Hi Richard,

    I work with both systems and I can tell you that this sort of operation is no problem in Creo.
    Admittedly, some 'special' options are somewhat hidden inside curve or surface features but it is all there.
    So, creating offset curves along a surface, normal to a surface (both parallel or variable), extending surfaces tangentially, normal or curvature continuous, copying boundaries or curve chains (here Creo actually offers better control about the the chain selection then CATIA, or to put it in other words, getting there with less features like extra points and splits), and everything that is trim (split), or merge (join) related works just as well as in CATIA, just different.
    For high end surface creation there is the style feature (a so called super feature which allows you to create free style curves and boundary surfaces 3 or 4 sided) in one feature.

    You might want to check the ATB (Advanced Topology Bus) in Creo which allows you to 'smart' import CATIA with the option to update the imported surfaces and curves in Creo if the CATIA model changes.

    If you have specific questions about feature comparisons, I am happy to assist.

    R
    rohit_rajan15-Moonstone
    15-Moonstone
    September 15, 2015

    your experience is older than Creo!

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      rpostak1-VisitorAuthor
      1-Visitor
      September 15, 2015

      Rohit,

      I got my first introduction to CAD in 1979.  Back then, 3D modeling was all wireframe and surfacing capablilities was very limited.

        R
        rohit_rajan15-Moonstone
        15-Moonstone
        September 15, 2015

        and i would be born next year 1980...nice talking to you Richard.

        R
        rpostak1-VisitorAuthor
        1-Visitor
        September 17, 2015

        How do you extract the edge curves of a surface and then do a paralell offset of those curves along the surface?

        D
        DG_8950681-Visitor
        1-Visitor
        September 17, 2015

        Hi Richard,

        select the curves_copy_paste_offset

        selecting chains can be tricky, if the curves are not continuous creo may fail to make the copy with no explanation as to why.

        select the first curve_copy_paste then shift click the chain in curve window works best.

        changing the curve type approximate can be helpful in joining a chain into a single spline

        ...but....it can also have some adverse affects

        C
        Constantin15-Moonstone
        15-Moonstone
        September 17, 2015

        One word on the 'approximate' option in curve copy.
        This will give a single segment spline as the result (which often is nice) BUT is only works if all elements are C1 or C2 continuous.
        In other words it will definitely fail, if there is a corner in the chain.

        R
        rpostak1-VisitorAuthor
        1-Visitor
        September 24, 2015

        Okay Folks,

        Another question for all.  How do I extend a surface along contour of the surface?  In CATIA terms, it would be "extrapolate surface".

        Regards

        M
        mpeterson1-Visitor
        1-Visitor
        September 24, 2015

        Select one segment of the surface edge to extend. Select the Extend feature and then you can continue to select more of the desired edge, but you need to select them by picking adjacent segments until you have the complete surface edge. If there are internal corners to this edge they might not extend. There are limitations to extending surfaces. In some cases where you have a jagged edge it might need o be trimmed first to extend it.

        R
        rpostak1-VisitorAuthor
        1-Visitor
        September 25, 2015

        Thanks...I got this to work for me, but like you said "there are limitations to extending surfaces".  I'm finding that out.  I was only able to extend my main surface by .75" and no more, but I was needing to extend it to about 6".  Is there a untrim surface function in CREO like there is in CATIA V5?

        R
        rpostak1-VisitorAuthor
        1-Visitor
        September 30, 2015

        All,

        I would like to take this opportunity to say "thank you" for all of your help with CREO.  My evaluation time has expired so I am no longer able to do anything.  Now it is up to the Configuration Management team to decide whether or not to go to CREO.

        Regards,

        Richard Postak

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