Help Needed with correct Plane alignment

[OldDogmeat]

Hello all,

I'm new here and am also new to SW but have a lot of past professional experience with various parametric and history based relational CAD and 3d modelling tools (Autocad + SME - many years ago, Autodesk 3D Studio, Maya, Softimage); so consider myself quite well versed in the thoery of 3D modelling in general.

I'm slowly learning SW but am finding certain aspects of the software quite awkward. I'm sure there are reasons for this and suspect it may be to do with the fact that the software is designed with real world manufacturing in mind and thus there being strict rules on solid and surface creation.

Anyway; I have a major issue atm with the alignment of a plane that I need orienting in a very precise way.

Here is a general overview image of what I am trying to achieve

http://i419.photobucket.com/albums/pp277/OldDogmeat/Image1.jpg

In the above image I have 4 lengths of square section tubing (25mm SWG-16); The top and bottom tubes are both parallel with the top tube set back in the side view; they are also both square to the world; These two tubes are then linked with the 2 side tubes which are both tilted back as well as tilted outward (bottom to top) to meet the top and bottom tubes at thier ends as can be seen.

I need the two link tubes to meet the top and bottom tubes aligned so that the profile edges are flush with the top and bottom tubes.

I hope that makes sense

The way I have attempted to go about this is to try and create an extrusion profile with the correct alignment by creating a plane that is normal or perpendicular to a line drawn as a path between the top and bottom tubes as seen here :-

http://i419.photobucket.com/albums/pp277/OldDogmeat/Image2.jpg

I have tried various (probably all) of the plane creation options; Normal to Curve, Through Lines/Points etc etc and nearly get what I am trying to achieve BUT the plane is slightly rotated on the splines pierce axis as shown here from a top view :-

http://i419.photobucket.com/albums/pp277/OldDogmeat/Image3.jpg

and so the resultant extrusion, set to bi-directional upto Surface gives me the following :-

http://i419.photobucket.com/albums/pp277/OldDogmeat/Image4.jpg

As you can hopefully see; the edges of the tube arent aligned with the bottom tube and it's obviously the same story at the top tube

Here's another view :-

http://i419.photobucket.com/albums/pp277/OldDogmeat/Image5.jpg

I'm sure there's a simple way to achieve this but I have spent hours trying all sorts of madcap ideas to try and create a plane that is correctly oreineted to allow me to create a simple rectangle that is aligned as required.

Apologies if I have missed anything obvious here or if my cry for help is a result of my lack of knowledge or understanding of SW.

If anyone can tell me how to go about doing this properly I would be extremely grateful.

Thanks in advance.

Dan

 

[TheTick]

There is no real effective way to control the rotation of a plane in SW. Horizontal reference tends to be arbitrary.

The next best thing to do is set up a reference to use as your "horizontal" or "vertical". Instead of using horizontal or vertical constraints, constrain perpendicular or parallel to your orientation reference.

 

[JMirisola]

Not sure how you're going about it, but here's what I did:

Offset a plane equal to the offset between the top and bottom tubes. Create a sketch line on each of the parallel planes. Create a 3D sketch between the endpoints of the two existing lines.
Use the weldments feature to create your top and bottom tubes first. Create one of the side tubes. You'll need to edit its sketch to get it to sit properly but, once done, you'll be able to mirror it over.

Hope this makes sense!



Jeff Mirisola, CSWP, Certified DriveWorks AE
CAD Administrator, Ultimate Survival Technologies
My Blog

 

[williedawg]

Don't think you'll get the edges of the side tubes to meet flush & align with the square cut ends of the horizontal tubes.

Imagine the horizontal tubes not in the model yet; only some planes that represent the vertical distance between them. Side tubes can be inserted as extrusions with a length in excess of those planes, then the planes used to cut/surface.
If a side tube is constructed perpendicular to those planes, (no side tilt) the ends will be square in any view.
So far, so good.
If it is then tilted back, the ends remain square as they were as viewed from the Front and angled when viewed from the Right.
The problem comes in when the side tube is (addtionally) tilted off to the side.

The cut egdes of the tube are still square in the Front view, still angled in the Right view, but; when you look down from the Top, the cut becomes a trapezoid (parallelgram?)

Once the horizontal tubes are placed in the model and some plane constructed at some point along a line connecting some feature of those tubes, 2 alignments may be satisfied, but not 3. Rotating the skecth perpendicular to said plane for the side tube may get it close, but it still won't come out aligned evenly with the squared-off end cuts of the horizontal tubes and the front/back sides of same.

Something has to give, angled end cuts on the horizontals or gaps/overlaps at the corner junctions

Make sense ?

 

[williedawg]

Rotating the skecth perpendicular to said plane for the side tube may get it close

meant to say "Rotating the sketch in said plane for the side tube may get it close"

 

[OldDogmeat]

Thanks everyone.

I'd expected the angled cut tube obviously to no longer be 25mm square but I hadnt imagined that with the two tilts it would effectively un-square the cut profile as seen from the top view.

Now that I think about it though it does make sense. Thanks for the explanation Willedawg; One of those things where you try and visualise it but with the 2 tilts and the resulting angled cuts accross the profile I was struggling to see what was happening.

Cheers
Dan

 

[OldDogmeat]

Sorry that first sentence makes little sense

What I meant was with the cut accross the profile I had expected the cut to no longer be 25mm square but hadnt expected it to become a parallelagram and was expecting some kind of rectangular section.

Thanks again everyone; Great forum.

Dan

 

[twinsemi]

For this type of construction, where you are working with distinct extruded contours, it is often easier to work with separate parts in an assembly to make the weldment that you are after.
1. You place the square and horizontal pieces into the assembly first, establish their relationships, and then add the connecting pieces.
2. Position the connecting parts using whatever relationships work best for you and then cut them to match the horizontal parts by either using an "in assembly edit" or measure the angles that you need and use those back in the part model.

By using multiple configurations of one part for each of the extrusions in the assembly, you are assured of having identical contours and the assembly won't modify those contours. (because it can't)

Tom Winsemius
Oxigraf, Inc.