Detailing Drawings

[solidhardhead]

Two detailing questions..

1.) Is there a way in my solidworks drawing to fix the arrow of a leader line to a part of my model so that when I change my model the leader will "follow the change" and remain attached to the item I want?

2.) Is it possible to mirror hidden lines that my model has created? Or do I have to manually draw them in?

Thanks Again!

 

[CorBlimeyLimey]

1) This should happen automatically when placing the note. If it doesn't, then before placing a note, RMB click on the view and select Lock View Focus. If the note is already placed, just dragging the arrowhead away from and then re-attaching it to geometry in the view should work.

2) Hidden lines are created from features which exist in the model. To show all hidden lines in a view, first select the view then select the Hidden Lines Visible icon in the View toolbar. An individual features hidden line detail can be shown by RMB clicking the feature in the View Manager then selecting Show/Hide > Show Hidden Edges.

 

[smcadman]

1. Put the leader endpoint on an edge of a feature, not the face of it, for it to move when modified.

2. Mirror hidden lines? Pardon me, but huh? The hidden lines are created automatically. If it doesn't have hidden lines, then you have hidden lines off or there aren't any lines to be shown. Why would you like to create hidden for something that isn't there? Please clarify.

SW07 SP2.0



Flores

 

[smcadman]

Sorry, not the first time it seems like I regurgitated an answer from someone else. I didn't hit refresh on here, so it looked like there wasn't an answer already.

SW07 SP2.0

Flores

 

[solidhardhead]

The reason I wanted to mirror a hidden line is because I am drawing the side view of a flange with boltholes. If I show the hidden lines in that feature it reveals every hidden line for every bolthole. I was hoping to just show two bolt hole hidden lines, one at the top one at the bottom. I am sure I can work around this problem by adding an additional hole to my model because right now I am only showing the bolthole of my original hole (prior to array). I was just wondering if there was an easier way that I may not know of.

Thanks for the fast reply

 

[solidhardhead]

don't worry I will take all the input I can get smcadman

 

[J-C]

You can show just the hidden lines for a feature(s). Expand the drawing view you are working in the feature tree. Find the feature in the tree, right click and "show hidden lines" .....or something like that.

If it still shows too many hidden lines....you could try some other things. If there aren't too many hidden lines...you can show the "Line Format" toolbar...there is a tool to hide and show model edges. Then hide the extra ones. Another technique is to toggle on all hidden lines...then select the hidden lines you want and use the "Convert Entities" sketch tool to extract the edge to a sketch line. Then use the Line Format Toolbar to make the sketch lines the hidden linetype.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP5.1 on WinXP SP2
SolidWorks 2007 SP2.1 on WinXP SP2

 

[CorBlimeyLimey]

You could also create a section view cutting across 2 bolt holes.

Or create Broken-out Sections at opposite bolt holes.

 

[fcsuper]

If you are close to your solution, but still have a few extra hidden lines, you should be able to right-click on them and select "Hide".

Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA

http://sw.fcsuper.com/index.php