hydraulic tube modeling

[fanoeng]

what is the easiest/quickest way for modeling hydraulic tubes? I have a hundred or more different tubes to model

I know the sweep but for a single plane only; I cant seem to get creo to continue the sweep if I want the geometry to continue onto a different plane. 

I can do an assembly. simple but not practical as i'll have more parts. 

the curve through points is a way but I'll have to learn it, just wondering if I should?

does the intersection way work? no not for a tube, maybe a hose. 

whats the most efficient way, guys?

[StephenW]

If you use the search in the upper RH of Creo, you can find the PIPE command. It's not in the ribbon and I don't think you can find it any other way but it does good job using points and you can set radii for the corners. The points would be at the ends of the pipe and at the intersection of the bends.

Applications - Piping if you have a license for the piping module is really the easiest way if you are doing piping from scratch.

Sweep would be my least favorite.

[fanoeng]

i tried making a part in piping but i came to the understanding, it had to be done in an assembly. 

[StephenW]

Correct, piping is an assembly function. I'm assuming they did that because it's really part of routed systems and you would be designing your pipe/hose runs in the assembly.

Depending on what your end goal is will dictate the workflow.

I usually create an assembly and then do each pipe in its' own assembly. Typically I would have the tubing and end fittings for the tubing so assemblies made sense.

[nhall]

I have just had a quick play and managed to get a tube-like shape using Swept Blend by creating a set of points relative to the coordinate system then adding a datum curve through the points.

You can then create planes perpendicular to the curve at each point by CTRL selecting both the datum curve and a datum point. Draw your hose section on each plane, where the datum point is the circle centre.

Create your swept blend.

Needless to say, the more points/sections you add the better the result but if you are just looking for visual effect then this could be a solution.

[TomD.inPDX]

I find that calling the 3D curve a datum feature is somewhat misleading... it is simple a 3D curve in my book.

It is worth learning how to use this feature.  Also look at intersecting 2 sketches to get a 3D curve.  Another option is to use edges such as a contoured surface.

Sweeps will fail at non-tangents.  A datum curve makes sure they are completely tangent unless you choose the sharp corner option within the set.

Keeping thing parametric while moving components is a bigger challenge.  All these techniques can be combined into making a comprehensive model with dynamic motion control.

[dschenken]

http://support.ptc.com/help/creo/creo_pma/usascii/#page/part_modeling%2Fpart_modeling%2Fpart_five_sub%2FAbout_Pipes.html%23

The alternative is a datum curve through points followed by a sweep. See http://support.ptc.com/help/creo/creo_pma/usascii/#page/part_modeling%2Fpart_modeling%2Fpart_four_sub%2FAbout_the_Curve_through_Points_User_Interface.html%23 for info on making the curve through points. Since is is a single curve it is easy to select it and create the sweep.

The first option is very fast. The second is slower, but - if poor choices are made in modifying a pipe feature it can be frustrating to fix it if it fails. With the second method there is nearly no chance the datum curve can fail in a mode that UNDO won't fix, and you can look at the curve to see if there is some place the pipe/tube/hose would not work (Usually a bend radius that is too small or a radius that eliminates a straight section.)