Change detail view circle to a detail view rectangle 1

[cadman64]

I'm trying to convert from AutoCAD to Solidworks. All our current detail views are rectangle because they're created in a viewport which is rectangle. How can I change Solidworks detail view circle to a rectangle? Is it even possible?

Thanks!

 

[grunt58]

sketch the shape you want (you can use any shape) then select detail view pick the sketch you just created the select connected then select profile.

see attatchment

we do these a lot sometimes a cirle doesnt show enough or shows to much.

Grant
Certified SolidWorks Associate
SW2009 X64 SP 1.0
Dell Precision T5400
Nvidia Quadro FX 5600
Xeon 2.5GHz Quad Core, 4GB RAM
XP Pro X64 SP2.0

 

[cadman64]

Thanks Grant,
I tried your suggestion and I'm not having any luck. To select "Connected" and then "Profile" isn't an option. "Profile" is grayed out no matter what "Style" I choose. I tried to edit the profile and create a rectangle scetch but when I click on the green check, it goes back to the circle. So neither of those two methods are working.

 

[fcsuper]

You can choose an enclosed rectangular sketch instead of a circular one. In old versions of SW, the detail region will still be a circle, but the detail view itself will be the shape of the sketch.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[grunt58]

Thats how to do it in 09. What version are you using?

Grant
Certified SolidWorks Associate
SW2009 X64 SP 1.0
Dell Precision T5400
Nvidia Quadro FX 5600
Xeon 2.5GHz Quad Core, 4GB RAM
XP Pro X64 SP2.0

 

[DesignerGuy16]

I've had issues trying to "make" the detail view as a rectangle. I usually end up making it as a circle. Right-click the detail view circle, edit sketch, delete the circle and then make a rectangle.

Doesn't give me any issues that way.

I think it has to do with rectangles in drawings don't necessarily mean a closed sketch like in a model.

James Spisich
Design Engineer, CSWP

 

[TheTick]

I just did this no problem. Just RMB the circle --> "Edit Sketch", then draw new outline.

The catch is that you have to have a segment of the new outline selected when you exit the sketch.

 

[fcsuper]

If you create the sketch and selete all of its entities prior to initiating the Detail command, there should be no issues.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[cadman64]

Ok, "the catch is that you have to have a segment of the sketch selected when you exit" worked. So I thank you for that. What it didn't do is change the detail view circle on the parent view. Is it possible to change that or at least hide it and stick a rectangle detail block over the top of it?

 

[TheTick]

Now you change the detail circle preferences to something besides "Per Standard" so that you can select "Profile" outline.

 

[cadman64]

Thanks, I got it. I appreciate your help. ;o)

Mike

 

[handleman]

One possible reason for problems drawing an initial rectangle:

If you start the rectangle outside the view boundaries, the rectangle entities will be put on the sheet rather than on the view. Entities "drawn on" the sheet rather than on a view can't be used for details, section lines, etc.

You only have to start drawing the entity inside the view boundary. Once you've started drawing the entity, the view boundary will automatically resize itself to enclose the new entities.

-handleman, CSWP (The new, easy test)

 

[cadman64]

Thanks for the tip. One more question, I've got my rectangle detail window, I put it on a layer to control the linetype and line weight, is there a way to save that to the document properties or incorporate that as the standard so that creating future detail views use those same settings?

 

[DesignerGuy16]

The only way I've had success with that handleman is when you create the rectangle, and while the rectangle is still selected, create the detail view. If you de-select the rectangle at that point and reselect the seperate entities it doesn't like it so much.

That's why I just create the circle first. Doesn't take much more time, and I don't have to worry about it acting up.

James Spisich
Design Engineer, CSWP

 

[takedownca]

Cadman,
The better way to control how the detail view displays is by editing the document properties on your drawing templates. You can select the shape, line thickness, and line font without resorting to layers.

 

[cadman64]

takedown,
Thanks for the tip, but I'm having a hard time finding where you can change the detail shape in document properties. Can you steer me in the right direction?

Thanks!

 

[DesignerGuy16]

After you've changed the detail view from a circle to a rectangle, etc. Click on the detail view itself. Select the style to be: With Leader. Then below that, select Profile instead of Circle.

Viola.

James Spisich
Design Engineer, CSWP

 

[takedownca]

cadman,
Sorry, I guess I was mistaken. I can't find an option to define the shape anywhere in the document properties either. However, there is a "Display new detail circles as circles" checkbox under System Options>Drawings. I don't think it does anything, though (might be a bug). Mine happens to be unchecked, but detail profiles still show up as circles.

 

[fcsuper]

Jspisich has answered the new question.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

 

[takedownca]

Matt,
By new question, do you mean how do you "change the detail shape in document properties"? It was already discussed how to manually change the profile shape on a case by case basis, but this unfortunately has to be done every time you make a detail view. I'm not aware of a way to change the default profile shape behavior - unless there is a drafting standard that has this set by default.