Dynamic Hose, Rope, Chains, etc and Flexible objects

Jose_4

Is there anyway to make dynamic hoses within assemblies that are able to flex bend and still hold the connecting ends together?
I am trying to use assemblies but it seems trying to make the hosing separately is fools errand. It seems I am going to have to basically assemble the whole thing in a part studio and connect the hosing there...but all my parts across multiple studios etc. 

philip_thomas

Jose - there are several parts to your questions so here goes;

Currently Onshape supports 2D splines. If it a natural assumption that at some time in the future we will support 3D splines.
If you want a 3D "spline" it can be done today by intersecting two extrusions from orthogonal planes to create the 3D edge you are looking for to sweep your cross section along.
Onshape supports 2 point splines - these are exceptionally useful as they are very well behaved over a large range of positions.
Onshape supports fixed length spline - awesome right! Add a parameter to define the lengths of standard hoses etc
Use the tangency controls to ensure that the 2 point spline is normal to the connection points at both ends - it works very well.
The concept of 'in-context' features is a little different in Onshape. Part studios are for creating geometry (including hose, pipe etc). Assemblies are for describing motion. To develop bent pipe or hoses, you would do so in part studios between two known positions. If you don't know the positions, measure them in the assembly and then create the geometry in the part studio.
Most CAD solutions today don't model chains (ie the individual links (unless you are designing chains)) - same goes for flexible parts. Using the advanced mate relations, you can create pretty much any mechanism you need (turning pulley A turns pulley B etc).

Its hard without specific examples to help you more. We are very appreciative of your support as Professional user. If you care to make an example problem public, I (and many others here) would be happy to help you. You are free also to submit a support ticket and as a Professional user, it receives priority attention.

Thank you.

philip_thomas

Jose - there are several parts to your questions so here goes;

Currently Onshape supports 2D splines. If it a natural assumption that at some time in the future we will support 3D splines.
If you want a 3D "spline" it can be done today by intersecting two extrusions from orthogonal planes to create the 3D edge you are looking for to sweep your cross section along.
Onshape supports 2 point splines - these are exceptionally useful as they are very well behaved over a large range of positions.
Onshape supports fixed length spline - awesome right! Add a parameter to define the lengths of standard hoses etc
Use the tangency controls to ensure that the 2 point spline is normal to the connection points at both ends - it works very well.
The concept of 'in-context' features is a little different in Onshape. Part studios are for creating geometry (including hose, pipe etc). Assemblies are for describing motion. To develop bent pipe or hoses, you would do so in part studios between two known positions. If you don't know the positions, measure them in the assembly and then create the geometry in the part studio.
Most CAD solutions today don't model chains (ie the individual links (unless you are designing chains)) - same goes for flexible parts. Using the advanced mate relations, you can create pretty much any mechanism you need (turning pulley A turns pulley B etc).

Its hard without specific examples to help you more. We are very appreciative of your support as Professional user. If you care to make an example problem public, I (and many others here) would be happy to help you. You are free also to submit a support ticket and as a Professional user, it receives priority attention.

Thank you.

Jose_4

So I need a hose with female connector on both sides to attach from point A to point B... This is a print of my current assembly.. doing the hose without having everything assembled is going to be a biatch in partstudio...unless onshape deforms the spline to connect between 2 fixed objects. 

adam_mercier

I'm interested in that too. But I would need to do it in an assembly because I have imported parts. There is a workaround to export/import my complete assembly and to derivate it into a part studio, then create the hoses. 

philip_thomas

Jose_4 - I started by trying to make my example way too complicated. Until we have 3D splines, your best bet is to derive all the start/end locations into a new (single) part studio and build the hoses there. You will probably use the workaround that Adam describes if this is an assembly. Each route (for simplicity) should be a series of planar sketch segments that you then sweep along. You may use lines, arcs and splines (as in my example). This is not ideal, but it is workable if you need to model hoses/pipes. There are newer/better works flows coming, but i don't want to tease you with screenshots now. 
Please feel free to ask any questions about this proposed solution.

https://cad.onshape.com/documents/6bc48c39c5a09028c4bf8b6e/w/64421617f25e9a184237ca3a/e/4dc8d1b527fa8b74b77800c9

jon_butler

Hello,

This last post was a year ago, but it perfectly describes what I need to do. Have the workflows to achieve this now been added?

Thanks

owen_sparks

Hi @jon_butler

I've not worked with this example but I'd check out a pair of featurescripts, the 3D spline (with a sweep of yout choice) or the wiring featurescript that may get there in one hit. 

Owen S.

jon_butler

Hi Owen,

Thanks for the reply. I am new to Onshape and the issue for me is that the parts I want to fit the hoses between are linked from parts libraries and don't exist in a part studio. So there is no way to get the geometry from the Assembly to a part studio to create the spline. 

Am I missing something, or can this just not be done in Onshape?

Best regards

owen_sparks

Hi @jon_butler

No problem.  The short answer is yes.  The last update but one brought us "In Context Editing" or ICE.  This allows us to take a snapshot of the state of an assembly and use that in a part studio to allow the design of parts that need such relationships.

I highly reccomend checking out @cody_armstrong 's webinar recording of ICE for a great introduction to OS's approach to the concept.

Having got some points in space in a partstudio (from the transfer of the assembly locations via ICE) then we'd join those points with either the wiring FS or the 3D spline and a sweep.

This is just my take.  Others with more experiance may well offer up other better methods.

Cheers,

Owen S.

jon_butler

Brilliant! Thanks Owen, that worked perfectly.
Cheers!

owen_sparks

Wooo, (with a side order of Hoo).

Glad to hear OS is bending to your will.

Cheers,

Owen S.