×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Sweeps on 3D sketches

Sweeps on 3D sketches

Sweeps on 3D sketches

(OP)
Before I put my fist through my monitor... I know this can be done, as I have done it in the past, but I'm apparently not remembering the special "trick" required.

I have created a 3D sketch, starting at the origin. I then create another sketch for my profile (a circle), again using a plane through the origin. I then hit the sweep function, pick the circle for the profile but every time I try to pick the 3D sketch as the path, nothing happens...

Any ideas?

Thanks...

RE: Sweeps on 3D sketches

Measure the distance between your profile sketch plane and your path curve.  There might be a minute gap which makes it not possible.  This shouldn't preclude selecting the curve for a sweep path, though.

Check your filters to be sure.  Perhaps try filtering for curves only.  That, and try picking the 3D sketch from the feature tree.

I could be the world's greatest underachiever, if I could just learn to apply myself.
http://www.EsoxRepublic.com-SolidWorks API VB programming help

RE: Sweeps on 3D sketches

(OP)
The path curve is coincident with the origin and the profile sketch was done on the "Right" plane, which passes through the origin. There is no gap there.

I have also tried to pick the 3D sketch from the tree as well... several times...

No filters help...

Thanks for the suggestions though...

RE: Sweeps on 3D sketches

Are you highlighting the "Path" selection box before selecting the 3D sketch path?

Try pre-selecting both the profile & the path before activating the Sweep feature.


Making the best use of this Forum.  FAQ559-716
How to get answers to your SW questions.  FAQ559-1091
Helpful SW websites every user should be aware of.  FAQ559-520

RE: Sweeps on 3D sketches

(OP)
I had tried reordering the profile before the path, that didn't work, and neither did changing the size of the profile (circle). I went all the way down to .001" with no results. :(

RE: Sweeps on 3D sketches

Legrand, I have that size monitor and res, still is havoc on my screen. As Scott suggested, it may be sutting into itself. It may be to small to see or find. Or the radii are too small.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site
FAQ371-376
FAQ559-1100
FAQ559-1091
FAQ559-716

RE: Sweeps on 3D sketches

(OP)
It is not cutting into itself, as I have tried several different profile diameters.

Not quite sure what this means though: "IS the 3D sketch actually in 3D space?"
How could it not be in 3D space?

RE: Sweeps on 3D sketches

remember to exit your sketch before using the sweep feature.
sounds simple, but went through it today with an associate.

¿)

To get the best from these forums read FAQ731-376 before posting

RE: Sweeps on 3D sketches

(OP)
Scott: I used a line, moving from one axial view to another (i.e. from X to Y to Z), so it should be in 3D space then... I think...

dsgnr1: I can't exit the sketch via a sweep, it will only allow me to exit via an extrusion... what does that say about my "3D sketch"?

RE: Sweeps on 3D sketches

Quote (Legrand):

I can't exit the sketch via a sweep, it will only allow me to exit via an extrusion
Huh!

Quote (dsgnr1):

remember to exit your sketch before using the sweep feature.

The Profile & Path must be seperate sketches.

Both sketches must be exited from (using the sketch icon) before activating the Sweep.

The Path can be a 2D or 3D sketch ... even a 3D sketch with the path drawn on one plane (2D) will work.

The Paths start point does NOT have to be coincident to any point of the Profile. However, it does have to be coincident with the plane that the Profile is on.

[img=http://img102.exs.cx/img102/7276/sweep9rl.jpg]

Can you repost a (smaller) image showing your Feature Manager?


Making the best use of this Forum.  FAQ559-716
How to get answers to your SW questions.  FAQ559-1091
Helpful SW websites every user should be aware of.  FAQ559-520

RE: Sweeps on 3D sketches

(OP)
Ok... here's the tree:


Sketches are speperate (why I had posted larger pics before). Planes are coincident.

If someone's really bored, they can look at the part here: http://www.meche.net/images/012965.SLDPRT

I'm just about to the point whee I'm going to do this with a bunch of seperate sketches...

RE: Sweeps on 3D sketches

Unfortunately I do not have SW2005, so cannot read that file


Making the best use of this Forum.  FAQ559-716
How to get answers to your SW questions.  FAQ559-1091
Helpful SW websites every user should be aware of.  FAQ559-520

RE: Sweeps on 3D sketches

I have tried working your file and it seems that the 3D sketch is corrupt in some way. I opened a new part and re-drew the 3D sketch and it worked fine.

I think that it is best to draw your path first then add a pierce relationship to the 3D sketch. It is much more stable than adding a coincident relationship.

Also I would try to add better contraints to your 3D sketch. There may have been something a little out of alignment causing the sketch to fail.

I hope this helps.


Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

Solidworks 2005 SP2.0

RE: Sweeps on 3D sketches

If you can't run a check sketch for feature then the sketch is corrupted. Try remaking the sketch.

Check sketch for feature is located under tools\Sketch tools\

Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: Sweeps on 3D sketches

Found something else... if you can't make this 3dsketch into a composite curve (which I bet you can't) You get the error "the sketch has disjoint segments and is not suitable for composite curve creation" then the 3d sketch is broken and that maybe another reason why the sketch will not be used in the Sweep feature.

Regards,

Scott Baugh, CSWP
3DVision Technologies

www.3dvisiontech.com
www.scottjbaugh.com
FAQ731-376
FAQ559-716 - SW Fora Users

RE: Sweeps on 3D sketches

(OP)
Oh My good glory.....
OK then... somehow, as you've found out, the sketch was "corrupt" (or disjoint, as SW loves to put it). I have never used the "repair sketch" funcion, and don't do much 3D sketching like this at all, but I think I'll remember this one!

I tried to create a composite curve, and, as you said, it errored on me with "disjoint sketch". I did the "repair in the sketch tools, and it's working!

Woot!

Thanks a million guys, sorry this one was so much greif.

Scott

RE: Sweeps on 3D sketches

Legrand,

I just tried your file, but I edited the 3D Sketch, and I ran the Repair Sketch tool (Tools->Sketch Tools->Repair Sketch) on it, then tried the sweep and it worked.  So something is definitly wrong with the sketch.  If it's not to late, give this a try.

Good Luck

RE: Sweeps on 3D sketches

Arrgh!  This is the second time I had to type this.  The site went down last time!

I tried making a composite curve of the 3D sketch, and I got an error message that the sketch was disjointed.  Maybe some endpoints don't quite meet or you have a segment doubled-up.

What's with the micro-sized straight segment in the middle of your hairpin bends?

I could be the world's greatest underachiever, if I could just learn to apply myself.
http://www.EsoxRepublic.com-SolidWorks API VB programming help

RE: Sweeps on 3D sketches

Eureka!  I found it!  Delete the first segment in the 3D sketch, and there is a second segment under it.

RE: Sweeps on 3D sketches

I should have remembered this from fighting with sketches before. Doubled lines is a common problem with imported geometry, too. To find and fix the double line (doppleganger?), drag to the left across each element. If there are two lines, then two will show up in the feature window list. Press "delete." Respond "yes" to one confirmation prompt, "no" to the other. Generally the first line in sequence is good, the next is the duplicate.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources