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Hide sketches one drawing view only

Question asked by Chad Huleatt on Feb 16, 2017
Latest reply on Feb 17, 2017 by Dan Pihlaja

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I need to show sketches on flat pattern view (bend lines etc). However, on the same drawing there are other views in which all the sketches should be hidden.

I have opened the parts/ assemblies and made sure that sketches are hidden there. (Using hide sketches, not going through the whole feature tree and hiding each sketch individually). However, the sketches still show up in the drawing view, and the only way to hide them is to select them individually.

I realise this question is similar to some that have already been asked. I have read those threads and the solutions don't seem to work, or are too labour intensive. Basically I want to hide all the sketches, except for the bend lines on the flat pattern. It should be easy to do that....

Thanks!

Glenn Schroeder Feb 16, 2017 5:05 PM

Correct Answer

In your Drawing, select the Bend lines. Then, while they're selected, use the Convert Entities function (on the Sketch tab of the Command Manager, or Tools > Sketch Tools > Convert Entities) to place sketched lines coincident with them. Now hide the sketches and the new lines will remain. You may need to use Layers or the Line Format toolbar to get the desired appearance on them.

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Jeff Parker Feb 16, 2017 4:58 PM

Once the drawing views have been created there is no link between the visibility of the sketches in the drawing and part. A macro would be the fastest option here, but you can also use the filter at the top of the Drawing tree to filter "Sketch" and then select all the sketches you do not want to see and hide them.

The last option would be to hide the sketches before hand and then create the drawing.

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Ingvar Magnusson Feb 16, 2017 5:03 PM

If you need sketches to be shown in the drawing e.g. for the flat pattern and have made some other views that sketches appear in. It is not enough to go the the part/assembly and hide them there. You need to hide them manually in the drawing or rebuild in the drawing and make the views again.

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Dan Pihlaja Feb 16, 2017 5:03 PM

Honestly, I would say that the easiest way would be to make sure that your sketches are hidden at the part level, then come back to the drawing and show the bend lines in the flat pattern view.

Alternatively, you can not worry about sketches at the part level, and hid sketches from the tree in the drawing.

I realize this will be hard if you have hundreds of sketches, but I don't know of a way to turn off sketches on a view by view basis. Only for the entire drawing or not.

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Glenn Schroeder Feb 16, 2017 5:05 PM

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Chad Huleatt @ Glenn Schroeder on Feb 16, 2017 9:16 PM

Thanks Glenn, that solves my problem. If you ever come to Australia I'll buy you a beer.

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Deepak Gupta @ Chad Huleatt on Feb 16, 2017 11:26 PM

I prefer and use what Dan has mentioned else the bend notes would hide too along with the bend line.

Further one can set the colors for the bend up/down lines according to the industry standards and with converted lines/new sketch you've have to change the colors manually OR use layer.

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Dan Pihlaja @ Chad Huleatt on Feb 17, 2017 7:47 AM

You and Dave Bear should hang out then.

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7 Replies

Jeff Parker Feb 16, 2017 4:58 PM
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Correct Answer
Once the drawing views have been created there is no link between the visibility of the sketches in the drawing and part. A macro would be the fastest option here, but you can also use the filter at the top of the Drawing tree to filter "Sketch" and then select all the sketches you do not want to see and hide them.

The last option would be to hide the sketches before hand and then create the drawing.
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Ingvar Magnusson Feb 16, 2017 5:03 PM
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Correct Answer
If you need sketches to be shown in the drawing e.g. for the flat pattern and have made some other views that sketches appear in. It is not enough to go the the part/assembly and hide them there. You need to hide them manually in the drawing or rebuild in the drawing and make the views again.
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Dan Pihlaja Feb 16, 2017 5:03 PM
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Honestly, I would say that the easiest way would be to make sure that your sketches are hidden at the part level, then come back to the drawing and show the bend lines in the flat pattern view.
Alternatively, you can not worry about sketches at the part level, and hid sketches from the tree in the drawing.

I realize this will be hard if you have hundreds of sketches, but I don't know of a way to turn off sketches on a view by view basis. Only for the entire drawing or not.
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Glenn Schroeder Feb 16, 2017 5:05 PM
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Correct Answer
In your Drawing, select the Bend lines. Then, while they're selected, use the Convert Entities function (on the Sketch tab of the Command Manager, or Tools > Sketch Tools > Convert Entities) to place sketched lines coincident with them. Now hide the sketches and the new lines will remain. You may need to use Layers or the Line Format toolbar to get the desired appearance on them.
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- Chad Huleatt @ Glenn Schroeder on Feb 16, 2017 9:16 PM
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  Thanks Glenn, that solves my problem. If you ever come to Australia I'll buy you a beer.
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  - Deepak Gupta @ Chad Huleatt on Feb 16, 2017 11:26 PM
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    Correct Answer
    I prefer and use what Dan has mentioned else the bend notes would hide too along with the bend line.
    
    Further one can set the colors for the bend up/down lines according to the industry standards and with converted lines/new sketch you've have to change the colors manually OR use layer.
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  - Dan Pihlaja @ Chad Huleatt on Feb 17, 2017 7:47 AM
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    You and Dave Bear should hang out then.
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Hide sketches one drawing view only

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