Fully Defined Sketches and Auto-Dimensioning in SolidEdge

[Phebotalus]

Hello.

I have used SolidWorks for a long time, but recently I changed workplaces, and SolidEdge is used. I'm still getting used to its finer details, and I had two questions:

1) Is there any way to tell when your sketch is fully defined/fully constrained/fully dimensioned? I know in SolidWorks it actually displays the text "Fully Defined" in a toolbar and your sketch changes colour, but it does not seem that in SolidEdge there is any way of telling.

2) Is there any way to automatically add all of the dimensions necessary to make a sketch fully defined?

Thanks a lot!

 

[donyoung]

Hi,

1) when in part/sheetmetal/asm
-- MainToolbar --> Inspect
activate 'Sketch Relationship Colors'
Tools --> Options --> General
activate 'Indicate under-constrained profiles in PathFinder'
(not available in ASM)

When in Draft and you have something to draw by yourself
activate Tools --> Maintain Relationships (it's off by default)

2) no, that's not possible in SE

HTH

dy

 

[Phebotalus]

Thanks a lot for your help donyoung.

 

[zaeka77]

I don't think that he is helping you but drowning you in a puddle.

Yes, this is possible .
1) Draw the sketch
2) Go to Tool->Dimensions->Relationship assistant
3) You can either make it show the items in the sketch which are not constrained and the number of dimensions required
OR
4) You select horizontal and vertical reference one after another and the selected items in the sketch are dimensioned automatically.
5) The type of dimensions to be used can be switched on and off from the options button on the Relationship assistant toolbar

Basically, read what the status bar says

 

[donyoung]

Hi,

I stand corrected but ...
you can easily guess from my comment to 2) that I never
did use that function for I don't have a need for such
a thing

dy

 

[donyoung]

/Edit

forgotten to mention is the 'Autodimension' function which
was introduced in V19. I use this function occasionally
but only in connection with keyed-in values.
Tools -- Intellisketch --> tab Auto-Dimension

dy

 

[KENAT]

Don's technique works fine for question 1, I'm not sure why zaeka77 disagrees. It doesn't tell you what's wrong though, which is where the option they give helps.

As to 2, auto dimension gets you part of the way but doesn't necessarily give you the dimensions in the way you want them.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?