Problem with sketleton sketch

[tchouk]

I invite anybody that will work with skeleton sketch to do that 5 minutes test, and try to understand what is going on.

1) Create a sketch (sketch 1) on the top plan in an assembly.

2) On that sketch draw a circle (5 “ dia.) That is coincident with the origin.

3) Draw a vertical line (line 1) from the center of the circle to the circle edge.

4) Draw a second line not vertical not horizontal (line 2) from the center of the circle to the circle edge.

5) Create an angular dimension from (line 1) to (line 2) set the angle to 90 degree.

6) Draw a third line (line 3) perpendicular but not vertical to (line 2) starting from middle point of (line 2), and a length of 3 “.

7) Now insert a new part in the assembly.

8) Mate the front plan of the part with the front plan of the assembly (coincident).

9) Do the same for the top plan of part and top plan of assembly.

10) Do the same for the right plan of part and right plan of assembly.

11) Edit the part in the assembly and create a sketch (sketch 2) on the top plan of the part.

12) Convert the entities (circle, line 2 & line 3)

13) Draw a point (point 1) on to the convert entity (line 3) and create a dimension from the point to (line 2).

14) Exit the sketch and exit the editing part mode.

15) Turn both sketches (sketch 1 & 2) to shown.

If you followed all the instruction you have now (point 1) that is located in the first quarter of a circle.
From the assembly double click on (sketch 1) and changed the angle dimension from 90 to 270 degree.
Rebuilt and ohhhh surprise (point 1) is know in the third quarter when it should be in the fourth quarter.
The proof: go back to a angle dimension of 90 degree (point 1 in the first quarter).
Enter an angular dimension of 271 degree, rebuild, (point 1) is know in the correct location in the fourth quarter.

 

[WorkingLife]

Hi Tchouk,

I've followed the steps that you provided and when I varied the 90 degrees to 270 degrees, like you said, the point is in the third quarter. Even at 271, I am still at the third quarter (which is what I would expect).

Maybe I am missing something, but I cannot see how it can be in the fourth quarter (my first quarter is top right, btw, and the fourth quarter is top left).

As you change the angle from 90 to 270, it would only move by 2 quarters (so from 1st to 3rd) since it's a rotation (and not a mirror function) of 180. So if the line3 points up, after a change to 270, the line is now pointing down.

If someone try this and have to same conclusion as tchouk, please let me know.

Allan Chun, CSWP

 

[TateJ]

I tried it - as best I could from your instructions - & it worked for me as I expected it should. I think you might be forgetting that line one was fixed vertical & the 90 deg dimension is working counter-clockwise. you'll see what I mean if you fix the second line horizontal - then make the other line perpendiculat to it (not vertical). Unless I mis-understood you... get ready to kick yourself for not seeing this. Happens to all of us brother... Don't sweat it.

Windows 2000 Professional / Microsoft Intellimouse Explorer
SolidWorks 2005 SP04.0 / SpaceBall 4000 FLX
Lava Lamp​

 

[tchouk]

Working life

Thank you for you comment
I made a mistake on my first message
At 90 degree the point is in the first quarter.
At 270 the point is in the fourth quarter.
At 271 the point is in the third quarter.
If you want I can send you the assembly.

 

[WorkingLife]

if you can send me the assembly, i wouldn't mind checking it out.

working_life@hotmail.com

Allan Chun, CSWP

 

[tchouk]

I found out the problem.
If you create the location dimension for the (point 1) from the point to the (line 2).
You get the point to be in the fourth quarter when changing the angle from 90 to 270,
or the point in the third quarter for 271 degree.

If you create the location dimension for the point (point 1) from the point to the (line 3)
The location of the point is the third quarter for 270 or 271.

 

[WorkingLife]

That is an interesting change in the point location (after looking at the file you sent me)

Like what you said, if you dimension from line 3, it will work correctly.

Allan Chun, CSWP

 

[CorBlimeyLimey]

Using SW04-SP2.1 that does appear to be a bug!

However, if you dimension from the end of line 3 to the point, (instead of from line 2 to the point) it works fine.

If you dimension from line 2 to the point, when line 2 is NOT horizontal (90° angle) it also appears to work ... until line 2 is made horizontal. The dimension then seems to pick up the horizontal constraint & "flips" when the angle becomes 270°.

SW2006 may have fixed this ... under some conditions, the dimensions in sketches are able to "flip" themselves correctly.


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