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ptc-53236611-Visitor
1-Visitor
April 24, 2014
Solved

detailing from .stp files

  • April 24, 2014
  • 3 replies
  • 5519 views

I have a doubt that is if we convert .stp file in to .prt file in pro-e........and after that i want to make a drawing of that prt file but i cant call any views,there are only two views standard and default orientation.but iwant to make orthographic views of that part or sub assembly or anything it is.............

Can anyone suggest me an answer


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Best answer by TomD.inPDX

You can also create new views by adding datum planes. You can either create datum planes based on geometry or the default coordinate system. You can also add planes using the import data doctor (edit definition).

once planes are established, you can create views to your heart's content. You can even create those views only in the drawing when you set up the view and not have ot save them in the model, however, that is the easiest way.

3 replies

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ptc-53236611-VisitorAuthor
1-Visitor
April 24, 2014

if any body didn't understand the question u can ask me back.............because the solution for it is very precious to me

D
dschenken1-Visitor
1-Visitor
April 24, 2014

Look in the help files for Saving Views and Orienting the model.

You can use Google to search for "Pro/ENGINEER Wildfire 3.0 Tips - U of M"

T
TomD.inPDX17-PeridotAnswer
17-Peridot
April 24, 2014

You can also create new views by adding datum planes. You can either create datum planes based on geometry or the default coordinate system. You can also add planes using the import data doctor (edit definition).

once planes are established, you can create views to your heart's content. You can even create those views only in the drawing when you set up the view and not have ot save them in the model, however, that is the easiest way.

    Mahesh_Sharma
    Mahesh_Sharma22-Sapphire I
    22-Sapphire I
    April 24, 2014

    Rajanarendra,

    You may try below options:

    1. Instead of directly opening a step file, create a part and import step in part using Model > Get data > Import > Import Step file. This will provide you all predefined views, whereas directly importing step will not give any views.

    2. Directly open the step file > It will import with a coordinate system and Import Feature ID in model tree > Drag "Insert Here" on top of "Import feature ID" > Click on Plane > It will create three datum planes. These planes can be used for View creation as suggested by Antonius.

    J
    JonathanHodgson13-Aquamarine
    13-Aquamarine
    April 25, 2014

    To create an orthographic set of views in the drawing, you only need to orient the first view correctly (which as mentioned can be done in a number of ways).

    You can then create projection views from the first view (and from each other) - there is no need to create a named view for every projection.

    T
    TomD.inPDX17-Peridot
    17-Peridot
    April 25, 2014

    I think the original request is to make the "right" starting plane where the original coordinate system was not oriented in the way they needed it.

    Now that I know this is a car body, I can see how one would want to orient the body for fixturing based on a common inspection plane.

    So yes, existing geometry can help create the basic 3 planes for the new orientation desired for continued development of fixtures and drawing orientation. physical flat surfaces or points can be used to define the primary plane, and the rest can follow normal from this one plane and a point. The 3rd of course is normal-normal to the 1st 2 and a vertex.

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