New FeatureScript: Hose Routing

sebastian_glanzner

Hello Everyone,

Good News! I'm releasing my Hose Routing FeatureScript:

https://cad.onshape.com/documents/54d06a3b8abd1fcb0daba26b/w/00a336bf184d3800f0194a5c/e/e689b647e557695970d3d603

The FeatureScript uses Arcs and Circles as input (either from solids or sketches).
You don't need sketches at all, which makes it more efficient if you want to create hose routings in context.

Usage:

1. Select the start of the hose
2. Select the end of the hose
3. Optional: Add midpoints between start and end (in the correct sequence)
4. Use the flip direction buttons if the assumed direction is wrong (only start and end)
5. Choose a hose size or use the "Custom Size" Button
6. You can also edit the straightness but normally this is not necessary

There are some cases the FeatureScript can't find the correct path for the hose:

• Try to use different "Mid points"
• Flip the direction at start/end if necessary
• Make sure the hose does not intersect itself

Thanks for the help, support, inspiration (Wiring FeatureScript ) and motivation:
@Jake_Rosenfeld
@ilya_baran
@romeo_graham392
@owen_sparks
@MBartlett21

lougallo

Nice job @sebastian_glanzner.  Might consider adding array parameters so you can nest multiple Hose routes in one feature.  Love this.

owen_sparks

This looks wonderful, I'm enthusiastic to try it out tomorrow, thanks for making it public.
Owen S.

michael_mcclain

@sebastian_glanzner Good work and I really like using this feature for flexible tubing or cable routing with certain types of cable.

Can I request some updates to it?

I would like to be able to re-order mid point selection similar to how the loft command has right now. It would be very useful for changing midpoints without having to clear the selection.

Regards, Michael

TimRice

@sebastian_glanzner should be able to use the

ALLOW_QUERY_ORDER 

UIHint to allow query reorder. To learn more please see the UI Hint section of our documentation:
https://cad.onshape.com/FsDoc/library.html#UIHint

sebastian_glanzner

@michael_mcclain

Thanks for the nice feedback. I am very happy that the feature is useful and hopefully saves a lot of time.
I think your improvement idea is very good! I have updated the feature! 

@TimRice
Thanks for the support, that was exactly what I needed. It helped me a lot 

michael_mcclain

@sebastian_glanzner thank you very much! And thank you to @TimRice for the help. That change makes the feature a bit more robust when facing downstream changes.

I have a question about the feature. Is there a reason why you can select the ID and OD of the tube, but the geometry only shows the OD? Does it create self intersecting geometry when it Calculates?

I think the feature is great and I end up using it a lot in my design work.

Regards, Michael

sebastian_glanzner

The ID is used only used for internal calculation of the density/mass.
When I developed it I also used the ID for the inner geometry but the sweep command was quite time costly.
This is the only reason. 

Can you share a screenshot of some your work?

MBartlett21

TimRice said:

@sebastian_glanzner should be able to use the

ALLOW_QUERY_ORDER 

UIHint to allow query reorder. To learn more please see the UI Hint section of our documentation:
https://cad.onshape.com/FsDoc/library.html#UIHint

@TimRice

Will this UIHint get added to the 3d fit spline command at any point? It would be very useful

Krz

@sebastian_glanzner Could you please add icon?

sebastian_glanzner

@Krz Icon added 

Krz

nice :-) It's easier to find it on the list now. Thank you

Jake_Rosenfeld

@MBartlett21

We actually did an audit this dev cycle to find features where selection reorder is useful, and added it in where appropriate. This will be released in our next release.  3d fit spline is included.

Jake_Rosenfeld

@MBartlett21

This has now been released for the selections we thought were appropriate.  Feel free to let us know if there are any we did not make reorderable that you think should be.

https://forum.onshape.com/discussion/12157/improvements-to-onshape-august-20th-2019

andres_dandler

@sebastian_glanzner  Thank you for the feature!  It is excellent.  Could I make a request, please?  We are routing some hoses, and it is important to respect a minimum bending radius.  This way, we can avoid the tubing from kinking.  Would it be possible to set a minimum radius for the hose routing?

Thanks again for an excellent feature.

sebastian_glanzner

@andres_dandler Thanks for the feedback! 

About the minimal radius:
I'm not sure how to solve this. I think I would have to start a query that finds the smallest bend radius of all splines.
I don't know if there is a command for this.

@TimRice
Is there a command to find the smallest bend radius on a spline?

TimRice

I checked in with our internal FeatureScript team and @paul_chastell suggests calling evCurvature along a number of samples on the curve to get the largest curvature. Then 1/curvature = radius of curvature. Keep in mind this is an approximation. @ilya_baran also mentioned you should check tangency along the curve to ensure you do not miss small high curvature sections.

lana

@sebastian_glanzner
FS does not have a way of finding min curvature radius, but there is evEdgeCurvatures, that you can call in multiple points and maximize curvature over that. You can do several iterations refining at promising areas. 

sebastian_glanzner

Onshape is able to calculate the min. Radius by showing the curvature, which is really cool!



Is there really no FeatureScript function?

sebastian_glanzner

@andres_dandler I made a big update for the feature! It took me longer than I expected, but it was worth it!

• You can set an custom minimal bend radius.
• This feature extracts the minimum bending radius of each segment.
• The smallest radius is displayed as info text when editing the feature.
• If a bend radius smaller than the "minimum bend radius" is found, a warning is displayed and the feature shows a red question mark.
• Any segment that violates the bend radius is also highlighted in red. 

@TimRice @lana
Thanks for your tips about the evEdgeCurvature :-)

TimRice

@sebastian_glanzner
I love all the UI/UX hints you added in. Nice work!

jonathan_monette

WOW great job Sebastian! very usefull

brucebartlett

i'll be giving this a tray thanks

owen_sparks

brucebartlett said:

i'll be giving this a tray thanks

https://youtu.be/Sv5iEK-IEzw

brucebartlett

Nice one! I won't edit, just for context. 

andres_dandler

Wow!  @sebastian_glanzner, this looks great!  I will give it a try.  Thank you so much!
  -Andres

sebastian_glanzner

@michael_mcclain

I have published an update of the FeatureScript. The inner surface is now displayed! 

Instead of sweeping a ring, which increases the regeneration time, I used the shell command, which is much faster!

victor_ragusila

awesome! this is really cool. For my project, a humanoid robot, we have hydraulic hoses routed around joints. I am trying to make sure they dont change length as I look at different joint positions.
I can position the joint however I want in the part studio using variables. Is there a way to specify length of hose, such that its length is kept constant at different positions?

john_mcclary

you can define the length of an arc or spline simple by adding a dimension.

victor_ragusila

Thanks, I used that previously and I was able to build a somewhat decent sketch for that...but it cant be in 3D, only 2D. My question was whether the point-driven spline from the Hose Routing FeatureScript release is able to also have a total length defined.

sebastian_glanzner

@victor_ragusila
At the moment, you can configure the straightness values manually to get the same length in each position.
I'm not sure how to do something like this automatically. 

I created a small example and I can see why it is necessary to have a constant length for each position