Sweeps from face to face (body to body)

[dubbed]

If you can imagine an A frame made out of tubing and trying to model the bridge in the middle without going through the tubings on the side but trimmed or mated to the face of them. thats what i can't figure out. someone help.

 

[CorBlimeyLimey]

If you are using the Weldments module, the end conditions are set with the standard options.

If it is not a Weldment;
Create a plane at the vertical centre of the 'A'.
Create the profile to be extruded in a sketch on the plane.
Extrude the sketch in both directions using the Up to surface option.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[dubbed]

oh right!
it is not a weldment, like the other parts of the model.
if only weldments included sweeps and lofts.

ok so start from the middle!

 

[CorBlimeyLimey]

The Weldments module recognises curves in the 3D sketches, so in effect it is doing a sweep. The "bridge" or cross-member could be a part of the weldment and could use a different profile from the rest of the 'A'.

What exactly are you trying to do? Can you give more detail and/or show an image?
See faq559-1100 for details.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[dubbed]

It's for a bike frame. I have two lofts / \ with ellipticle profiles and want to create a small bridge between the two /-\ . i was originally sketching a profile in one of the lofts and sweeping it to the other but created the extra pieces inside the lofts. what you suggested makes more sense and better suited for what i want to do.

i thought i tried weldments in a similar situation with no success. but you're saying i should be able to if the sketch is a 3D sketch? and then be able to trim to the lofts?

I'm at work so I can't post an image right now.

thanks!

 

[CorBlimeyLimey]

The Weldments module works with 2D & 3D sketches and with combinations of both.

You would need to add the elliptical tube as a custom profile.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[CADGemini]

dubbed,

Go here

http://www.mytempdir.com/967903

to download a file in SW06 format. I think this is what you are looking to do except that you will have to create the custom profile as CBL had suggested. Also do a search within solidworks help for "weldment profiles" to learn more.

To create a weldment profile:

Open a new part.

Sketch a profile. Keep in mind that when you create a weldment structural member using the profile:

The origin of the sketch becomes the default pierce point.

You can select any vertex or sketch point in the sketch as an alternate pierce point.

Close the sketch.

In the FeatureManager design tree, select Sketch1.

Click File, Save As.

In the dialog box:

In Save in, browse to <install_dir>\data\weldment profiles and select or create an appropriate subfolder. See Weldments - File Location for Custom Profiles.

In Save as type, select Lib Feat Part (*.sldlfp).

Type a name for Filename.

Click Save.

Best Regards,
Jon

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

http://solidworks.carbonmade.com/

Solidworks 2006 SP4.0

 

[dubbed]

thank you all

i saved a jpeg on my home pc but forgot to upload it.
I extruded from the central plain in both directions up to the loft surfaces. i'll work from there.

weldments did work but i was not able to trim afterwards. it would not select the lofts that i wanted it to trim to. maybe if I draw it short and extend to the lofts. but it seems you can only trim and extend from one weldment structure to another.

 

[CorBlimeyLimey]

Any particular reason you are using Lofts?

I haven't tried, but you may be able to create & use a zero offset surface to use as a trim tool.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

SW2006-SP5 Basic ... No PDM​

 

[SBaugh]

There is a trim option in the WEldments and you can use bodies, etc... but I suppose you have to have other weldment bodies to trim too.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[dubbed]

ok this is what i was doing.

i just extruded to surface.

http://burgerkingdude.googlepages.com/roadframe54disc1.jpg