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Tutorial: How to use Style command in PTC Creo Parametric?

Tutorial by Mohit Saxena
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Tutorial: How to use Style command in PTC Creo Parametric?

  1. Step 1:

    Step 1:
    The interface for style command is little different, as we open style command we see one of our datum plane is shown with grids. This plane is called active plane (means it is selected). Also in model tree we will only see style 1 as command name. Style has its own tree Style tree, below model tree. All the work that we do in style will be shown in style tree.

  2. Step 2:

    Step 2:
    Also we see that the in graphics toolbar also has five new options. The first one is style display filters

  3. Step 3:

    Step 3:
    The second is show all views which tiles our window to show four views

  4. Step 4:

    Step 4:
    Active plane orientation, orients the active plane parallel to screen just like sketch view command

  5. Step 5:

    Step 5:
    Show next view

  6. Step 6:

    Step 6:
    Visual mirror which displays the mirror image of our object about the selected datum plane

  7. Step 7:

    Step 7:
    In ribbon we see a command Set active plane, just click on this command and select the plane you want to activate

  8. Step 8:

    Step 8:
    Now in style the first command is Curve, click on it

  9. Step 9:

    Step 9:
    There are three types of curves, select the first option Create a Free Curve

  10. Step 10:

    Step 10:
    Draw your curve just as you will draw a spline and click ok

  11. Step 11:

    Step 11:
    To edit this curve just double click on it or select curve edit from ribbon

  12. Step 12:

    Step 12:
    You can edit the curve using control points like spline in sketch. You can add control points anywhere you like by right clicking and selecting Add point option. You can also add a control point in the mid of two control points using Add midpoint option

  13. Step 13:

    Step 13:
    If you try to move the control points normal to the plane you will see that your curve is now a 3D curve

  14. Step 14:

    Step 14:
    Next option is Create a planar curve

  15. Step 15:

    Step 15:
    It is drawn similarly like a spline

  16. Step 16:

    Step 16:
    Same ways to edit the curve

  17. Step 17:

    Step 17:
    But this curve will not be converted to a 3D curve, it will remain on the plane

  18. Step 18:

    Step 18:
    Next option is Create a curve on surface

  19. Step 19:

    Step 19:
    When you click on this option references will turn red, click on it. Then click on click here to add item and draw your curve just same way as the above two.

  20. Step 20:

    Step 20:
    Now draw a sketch like this forming a T shape and then select style command

  21. Step 21:

    Step 21:
    Select curve and choose Create a Planar Curve option

  22. Step 22:

    Step 22:
    Now draw a curve connecting the three end points as shown, for connecting the curve at the end press shift and then click at the end of the line. It will snap to the end, draw your curve and click on OK. If your end is connected it will display a circle otherwise a dot

  23. Step 23:

    Step 23:
    Now go to curve edit by double clicking on the curve and adjust the shape of your curve and click on OK

  24. Step 24:

    Step 24:
    Now we will create a plane parallel to this plane, click on the internal plane option

  25. Step 25:

    Step 25:
    Internal plane option is same as the plane option that is used to create a new datum plane. Create the plane and select curve option from the ribbon

  26. Step 26:

    Step 26:
    Now on this new plane draw another planar curve as shown using shift at the corners. But we see that our endpoints didn’t snap on our reference sketch. Not a problem just click on OK for now

  27. Step 27:

    Step 27:
    Double click on curve to enter curve edit mode, hold one endpoint pressing shift key and move it a little towards our reference sketch and will snap on it. Do same thing for the other corner and click on OK

  28. Step 28:

    Step 28:
    Now click on Set active plane from ribbon and select the plane normal to our used planes upon which our end points for both curves lie

  29. Step 29:

    Step 29:
    On this plane draw a planar curve connecting the two ends and edit its shape as shown below,
    When the end point will connect to another curve it will show a cross (X)

  30. Step 30:

    Step 30:
    Similarly draw a curve on the second side and edit its shape

  31. Step 31:

    Step 31:
    Now select the surface from the ribbon

  32. Step 32:

    Step 32:
    Press ctrl and select all the four curves one by one, if all your curves are connected end to end you will get a surface. Click ok

  33. Step 33:

    Step 33:
    Again click ok and come out of style command, you can perform all the surface operations on it in part environment

  34. Step 34:

    Step 34:
    For example try to mirror it

  35. Step 35:

    Step 35:
    Now merge these two surfaces

  36. Step 36:

    Step 36:
    Now right click on style 1 in model tree and click on edit definition. In style make this plane active

  37. Step 37:

    Step 37:
    Draw a curve from one end to another as shown below

  38. Step 38:

    Step 38:
    Double click on the surface to go to surface edit

  39. Step 39:

    Step 39:
    Click on the second option in the ribbon which says click here to add item or right click in the graphics window and select internal collector option and select our newly created curve, the surface will take the shape of the internal collector curve

  40. Step 40:

    Step 40:
    Now return back to part mode

  41. Step 41:

    Step 41:
    Use Thicken command and provide thickness to the surface

  42. Step 42:

    Step 42:
    Now we have a solid on which any operation can be performed

Comments

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    Nebojsa

    Great tutorial

    August 23rd, 2017 15:49