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cjohansson-21-Visitor
1-Visitor
April 28, 2014
Solved

Sketch to drawing

  • April 28, 2014
  • 6 replies
  • 11363 views

I have made a cut in the model, see image.

In the drawing I would like to use the construction circle diameter 70 to show where the 3 small holes are located.

I would also like to show the mid axis of the 29 dimension.

Can someone tell me how to do?

ScreenHunter_66+Apr.+28+13.30.jpgScreenHunter_67+Apr.+28+13.30.jpg


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Best answer by jzhang-3

Never sketch in drawing!

The most of simple way of showing dimensions in drawing is to add Geometry points in model sketch, and then add dimensions by measuring these points in drawing. These dimension are from model and will never broken (purple color). you can hide these points if you like clean views.

6 replies

J
jsarkar1-Visitor
1-Visitor
April 28, 2014

You can make draft datum or axis in the drawing by drawing references from model from the annotation tab. also you can add construction circle or entity etc from the sketch tab and try relate to view so the it keeps moving with the related views.

C
cjohansson-21-VisitorAuthor
1-Visitor
April 28, 2014

I´m quite new to this, moving from SolidWorks.

Can you be a little more clear, cause I do not see how you mean..

V
vmráz12-Amethyst
12-Amethyst
April 28, 2014

Generaly:

1) Drawing SHOWS information from MODEL ---> all information must be included in model.

2) Make some adding sketches in drawing is WAY TO HELL.

See attached pictures:

Model space:

01-model.JPG

Drawing space:

"CALL" dimmensions/axes from model.

02-drawing.JPG

C
cjohansson-21-VisitorAuthor
1-Visitor
April 28, 2014

Yes, I have understood that possibilities in drawing mode are very limited compared to SolidWorks.

So still do not see how to make sketch segments visible in drawing.

Diameter 70 in my images.

J
JonathanHodgson13-Aquamarine
13-Aquamarine
April 28, 2014

As far as I know you cannot make elements from a sketch that is used to create geometry visible in the drawing.

What I sometimes do is to create a separate sketch in the model, that references the geometry or the original sketch, showing only the lines I require on the drawing. I then create a new layer just for this sketch, so that I can hide it in all views except where I want it to appear.

For holes on a pitch circle, however, if you create the first hole and then axis-pattern it to create the others, it should be possible to show the correct axis and pitch circle elements automatically.

I agree with Vojtech that sketches in the drawing are always best avoided - generally they lose their parametric references and become detached from the geometry.

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cjohansson-21-VisitorAuthor
1-Visitor
April 28, 2014

Ok, thank you for your answer.

For me it is not a straight forward way to create a sketch, add to layer, hide layer.

I guess it will take a while for a SolidWorks user to learn how to goaround all drawing limitations.

    G
    GabrielZaha14-Alexandrite
    14-Alexandrite
    April 28, 2014

    In your drawing options you need to set the radial_pattern_axis_circle option to yes.

    To open the drawing options in Creo 2 selec File / Prepare / Drawing Properties. Then on the "Drawing Properties" dialog box select "Change" on the Detail Options line.

      J
      jzhang-31-VisitorAnswer
      1-Visitor
      April 28, 2014

      Never sketch in drawing!

      The most of simple way of showing dimensions in drawing is to add Geometry points in model sketch, and then add dimensions by measuring these points in drawing. These dimension are from model and will never broken (purple color). you can hide these points if you like clean views.

      T
      TomD.inPDX17-Peridot
      17-Peridot
      April 28, 2014

      For your paticular request, you want to change the hole axis to show the bolt circle axis.

      Then you can extend the two you are concerned with through the 29.0 features.

      Set this in your detail.dtl file (drawing options, not config.pro)

      radial_pattern_axis_circle YES

      You will have to pattern the hole features to make this work for you.

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