Sweeping Question??? 1

[quest4k]

Good morning, I have a sketch with a line and it is piercing one end of a single loop helix and then another line pierces the other end of the helix. Then I drew a fully defined circle on the end of the first line an tried to sweep the entire profile, but SW can not do it. It can only be done if I make three separate circle profiles and sweep one section at a time. Right now this is just a pain, but when I get to the complex bent tubes, it will be a nightmare, not to mention if an engineer makes a change in the tubing dimensions. The million dollar question, is there a way to sweep the entire profile in one pass? Thank you are any help rendered.

 

[Heckler]

Are these lines construction or solid? That might be your problem. You should be able to sweep a single section along a curve.

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
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford

 

[CorBlimeyLimey]

Convert the Helix into a 3D Sketch, then add the lines at each end within the 3D sketch. The profile should then be able to be swept along the 3d sketch.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[quest4k]

Thank you for the suggestion CorBlimeyLimey, but How do I convert this helix? Thanks again.

 

[SBaugh]

They have to be separate sketches to work CBL's suggestion will work for a workaround, but you should not continue to do these as a normal procedure.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[quest4k]

Thanks for the response, Scott. But there only three parts in the profile and I have not yet figured out CBL's suggestion and I have wasted about twelve hours playing games with this model and its' drawing and I can't get it even close to the correct output. I don't even want to see the complex bent tubes. Thanks anyway I think I am just going to give up and turn it in as is.

 

[Heckler]

Quest4k,

post an image of what you're after. I find it hard to believe it's a software limitation because I'm modeled exhaust manifolds with no problems. Please give us as much information as possible so we can try to help you. That's what we're here for.

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
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford

 

[SBaugh]

Start a 3D sketch, pick the Helix and Convert, that all you need to do.

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[quest4k]

Thanks for the response, Heckler, but I am not sure how to post the model, there is no attach here.

 

[Heckler]

faq559-1100 & faq559-1177 are great resources. In fact, I would take a look at all the FAQs so you know what knowledge base is available for free.

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
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford

 

[quest4k]

I think I got this right, I hope:

http://img530.imageshack.us/img530/2144/bt854wv.jpg

I hope this is right, well this is the easy one, so it has a one loop helix and two lines one pierceing each end of the helix. It is tube and I get many different sizes and bend designs. Some have several helixes and bends in them. This one that you see has three profiles in it, one for each section. I used just a standard sweep to make this. Thank you again for the help.

 

[SBaugh]

YOu want to make it more complex.

Take the helix and two lines and make it into a Compsite curve then sweep the profile and the composite curve.

You can find a model on my website like this "composite Curve"

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[quest4k]

Thank you Scott, I will give it a try in the morning. No, I don't WANT to make it more complex, but many of our customers have engineers and those engineers seem to have nightmares and they create these elaborate bend designs for what ever they are trying to do and lucky us we get to bend them and solder a bunch of things on them and ship them to the customer. Most of those designes make this look kid child's play and I get to make the model and drawings for it. Thanks again for the help.

 

[quest4k]

Good morning, Scott. Well I tried what you suggested and I even did it with a new profile and everything is fully defined. When I went to sweep the compoite curve, I got a warning message:
"Sweep resulted in topologically invalid body"
Any thoughts on this one? Thank you again for the help.

 

[quest4k]

I just discovered something. It is the off-set that is causing the trouble. If I sweep simple circle it works fine. If I use the off-set to I get the error. Is there any other way of changing this from solid to tubing? It has a .312 OD and a .065 wall, if that matters. Thanks again.

 

[CorBlimeyLimey]

Use the Shell function after doing the sweep.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[quest4k]

Actually the thin feature in sweep worked. Thank you one and all for the help.