cad to solidworks

[Corby]

Hi all I wonder if anyone can help, my name is Kev and I have imported a 2d autocad drawing into solidworks my problem is I cannot fully constrain the sketch( I have an Inventor background forgive my termanology)Icannot get the sketch to turn black i seem to ae able to add dimension everwhere and still not constrain it, I have no control over the sketch.
Hope you lot undferstand my question, Thank You

 

[smcadman]

Without seeing the actual sketch, we can't tell you exactly what the problem is. Besides dimensions, make sure the horizontal lines have horizontal constraints, the vertical lines have vertical constraints, etc. If there are radii, then maybe you are missing tangent constraints. Also don't forget to constrain the sketch to the origin.

SW07 SP2.0

Flores

 

[Heckler]

Depending on who created the A-CAD drawing, I have come across some sloppy drawings. For example, drawings that have line elements on top of others segments. I would go back into A-CAD to check for these types of errors. Depending on the complexity of the section you may want to consider just redoing the part instead of importing.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[CorBlimeyLimey]

If you have SW07 you could use the Sketch Xpert function to troubleshoot for you.

 

[Theophilus]

You'll need to pin an element of your sketch to the origin using a dimension (probably need at least two of these), or make a point in your sketch coincident with the origin.

I'd recommend reading the tutorials in SolidWorks before going too far so you optimize your models for logical flow of thought as soon as possible (and save yourself later headaches of having origins and primary planes in strange places within your parts and assemblies).

One thing I often do is draw construction (center) lines through the origins and dimension to those lines--horizontal and vertical. Dimensioning or constraining to the origin is what gives your sketch an "absolute" position, and therefore locks it down and turns black.



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[Theophilus]

Wow--four posts, four seconds. Now that's service!



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[CorBlimeyLimey]

You could also try the Tools > Dimensions > Fully Define Sketch function.

Or the Tools > Sketch Tools > Repair Sketch function.

Failing both of those, post the sketch for review. See faq559-1177 for details.

 

[CorBlimeyLimey]

Errr ... those are minutes Jeff!

 

[Corby]

lol what a great forum , im clad I joined what a speedy responce, thanks guys, will will give back to the community with my help from my field of autocad and inventor, enought of that, yes il read up pn the tuts, and you hit the nail on the head guys, normally i would sketch from an origin but when you import a cad drawing it just throws it anywhere it likes in space. I need to fit it to an origin ( i think) lol

 

[Corby]

Ill give that ago CorB, cheers

 

[JMirisola]

One recommendation:
As you beging to use SW more often, I've always found it easier to create my sketch/part centered around the origin. This will ease the creation of mates when you start creating assemblies, IMHO.

Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP2.0, Dell M90, Intel 2 Duo Core, 2GB RAM, nVidia 2500M

http://designsmarter.typepad.com/jeffs_blog

 

[Corby]

thats whats happened here autocad has placed the sketch about 500mm away from the origin, CorB suggested to workarounds, the first (FULLY DEFINE) did turn it black but I cannot update the sketh(edit it) the second REPARE SKETCH showed up the origin being way over there (about 500mm away quess) I think I need to now get the sketch over to the origin.

 

[JMirisola]

If the sketch isn't fully defined, you should be able to select it all and move it...just remember ctrl+z, in case it deforms.

Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP2.0, Dell M90, Intel 2 Duo Core, 2GB RAM, nVidia 2500M

http://designsmarter.typepad.com/jeffs_blog

 

[CorBlimeyLimey]

When using the Fully Define Sketch" tool, pick an origin point in the sketch itself ... not the main origin. This will fully define the sketch elements to the chosen point, but you will be able to drag the whole sketch onto the main origin without fear of mangling the sketch.

 

[dgowans]

Another method of dealing with sketch geometry that is way off in space relative to the origin:

1) Pick a significant point in the sketch and lock it down with a Fixed constraint. This effectively becomes the "sketch origin".
2) Constrain everything else so that the sketch is fully defined.
3) Delete the Fixed constraint
4) Add a coincident constraint between your sketch origin and the global origin. Alternatively, you can drag the sketch origin on top of the global origin to constrain everything.

This has worked for me in the past when dealing with imported sketch entities. This assumes that the sketch entities are clean as far as SWX is concerned.

 

[Corby]

yep it deformed lol. just not a big sketch its a simple bracket, the commandd I anm looking for is (in Inventor) COINCIDENT the move the sketch to an origin and allow you to fully define the sketch

 

[Corby]

Cheers dgowans I will give that ago now

 

[Corby]

where do I find coincident constraint I bet its in a toolbar I have not opened??

 

[Corby]

found coincident

 

[Theophilus]

If you select two elements of the sketch, you should see your feature manager turn into a constraints dialog where you can select Coincident, Concentric, Tangent, etc.

CorBlimeyLimey, you're right--those were minutes, not seconds. That means the service is only 1/60th as good as I thought--bummer! This demands another coffee. Back later. ..



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.