8 Replies Latest reply on May 21, 2013 11:39 AM by Dave Krum

    have a few questions with simple drawing

    Dave Krum

      Hello again all,

      I'm having a few problems with a simple drawing sheet that hopefully someone can answer.  I'm still learning .


      1. I know that with Autocad, two arcs cannot be dimensioned to an angular value for obvious reasons and I'm guessing that there is similarly no trick in SW to make this happen.  I was trying to somehow get an approx. angle at the vertex of the bent part.  I ended up just eyeballing two construction lines overlayed on top of the solid lines and just picking those two for an approx. angle.  Is this the best way?  I just put in an "~" in front of the angle.


      2.  When trying to pull an enlarged detail from this same vertex area, for some reason the detail is showing up way off the sheet and I cannot move it back onto the sheet.  The annotations that go with the detail show on the sheet but not the detail itself.  Cannot figure this one out.  Just avoided the detail all together.  Maybe I'm missing a step when I click "Detail View" and then draw circle and place the view on the sheet. 


      3.  When bringing in a new view to drawing (the flat pattern in this case toward lower left of sheet), in order to fit it in, I had to stray from the sheet scale to make it fit which is fine but SW isn't throwing a scale in with the view automatically when dropping it on sheet.  Does this need to be put on manually with the "note" annotation?


      4.  From reading on here, the only way that I saw to make a simple leader line to go from one place to another is to use "Insert / Annotation / Multi-jog leader" and just click the start point then RMB and choose end.  But this puts another arrow on other end of line and I'd like just the beginning arrow (such as in Autocad when using the leader line dimension).  You can see the 2 places where I used multi-jog but its putting double arrows.


      5.  Why are some of the dimension lines showing up in green?  Ever since I brought the Autocad flat pattern view onto the sheet, stuff started turning green.


      Thanks for any suggestions!  I'm only attaching the .slddrw file, hopefully the .sldprt files are not necessary.Untitled.jpg

        • Re: have a few questions with simple drawing
          Glenn Schroeder

          1.  You can create relations between the sketched lines and your arcs to minimize the eyeballing.  Other than that, I don't know of a better way.


          2.  I use Detail Views on almost every project and I have never encountered a situation where I couldn't move the Detail View.  I don't know what to tell you on this one except to duplicate the situation and then post the drawing and part here for someone to take a look at.


          3.  Yes, you will need to add this note manually, but you can link the note to the view scale so that it will update if you change the scale.


          4.  If you only want to change the location that a leader is pointing to, just click on the leader to highlight it, then click and drag the blue box at the end of the leader.  If there is a notation that doesn't have a leader and you want one, click on it to highlight it and there is a box in the PropertyManager that you can click to add a leader.  Then click on the end of the leader to place it.


          5.  They're probably in a layer that's green.


          And yes, when posting a drawing the part/assembly files are also necessary.

          • Re: have a few questions with simple drawing
            John Burrill

            Hi Dave,

            tackling your issues one at a time:

            1) you can dimension the angle included in any three points, if that's the start, common center and end of two arcs, there you go.  To dimension the angle of the arc where you placed the curve-length dimension, start your dimension tool, pick the right-end, then the center point, then the left end

            2) The only thing I can think of with your detail view, is that you don't actually have the parent view activated and locked when you place the circle.  Try double-clicking inside the view boundary before creating your circle.  the view will highlight and show brackets on the corners

            3) I'm assuming you have an annotation in your title-block that reports the sheet scale and you're tyring to get that to read the view scale.  OK, the best solution is to change your sheet scale to match your view scale and tell your view to use the sheet scale.  RMB on the sheet tab and select 'Properties' to pull up the sheet properties dialog.  change your scale to your view scale, click OK and then   change the view to use the sheet scale by picking inside its boundary and in the property manager that displays, populating the 'use sheet scale' radio button

            That's assuming you're only going to have this one view.  If you want to tag the view with a scale then you're going to do something similar to inserting a field in AutoCAD.  STart the 'create note' tool, locate the note inside the view.  type in the text surrounding your scale value (e.g. "SCALE:") and then select 'insert custom property' from the property manager.  Set the context to current sheet using the radio buttons and then pick the 'View scale' property from the list.  That will create a view tag that updates automatically when the view scale changes

            4) Unlike AutoCAD, solidWorks notes all have leaders.  The only question is whether you can see them or not.  So if you click on any note, you can turn on the display of leaders in the property manager.  Now, if the note was created without a leader, the arrow point will show up under the note text, but there's a grip that you can use to reposition it.  Leaders are associative to views, so make sure the view you want to place the note on is active.

            In your case, what you might want to do is add the 'to the inside of the bend line' to the arc-length dimension.  Pick the dimension and you can type the text around the dimension tag in the property manager, similar to what you do in the mtext editor in AutoCAD.

            5) My guess is that your imported dimensions are green because they were created on a layer in AutoCAD that was green and that layer happens to be current.  change the layer back to 'per standard' or 'none' to draw with the default symbology.

            I tried looking at your drawing, but you didn't include the part files, so the views came up empty.  Anyway, try working those points and let us know how it turns out.