assigning a value to arc length

[BertilRogmark]

I am working in WF3.

I have a part in an assy. The part is a hose connecting 2 points in the assy, on fixed and one on a another part that can move within certain limits. I want to make sure that the hose will adapt its bending curve to achieve this but you have to remember that the hose must have a fixed length and only the bend angle and the radius an vary.

If I could lock the bend arc length to a set value it would be easy.

Fixing the hose to its known start and end points, locking the value the length of the straight (not bendable) ends I only need to lock the arc length.

I can measure the arc length but have not been able to find a way to lock this value.

Help!

[vnamboodheri]

Hi @BertilRogmark,

Thank you for your question. 
I’d like to recommend to bring more details and context to your initial inquiry. 

It also helps to have screenshot(s) to better understand what you are trying to do in your process. 

This will increase your chances to receive meaningful help from other Community members. 

Regards,

Community Moderation Team.

[BertilRogmark]

Hope this makes it clearer:

This screendump shows 2 rigid rods, length 100 and 165 respectively, connected by a flexibel hose.

The rigid rods are fixed to PNT1 and PNT0 respectively.

I want to assign a fixed value the the length of the flexible part in order to see how the curve changes when I move PNT0 in relation to PNT1.

I can calculate the arc length using the perimeter type dimension but I have not found a way to assign a value in a relation.

[tbraxton]

If I understand the problem statement correctly, then this should provide a sketch that will define the range of geometry within a limited range.

[FriedhelmK]

It would also be particularly helpful if you asked your question in the right forum.
>I am working in WF3.
Does WF3 stand for Wildfire 3 ?
pro/engineer-wildfire and Pro/ENGINEER is now Creo Parametric.
I can't tell you where you should ask your question, in any case here you've come to the wrong place.

[BertilRogmark]

I thought everybody knew that PTC earlier used the name Proengineer and Wildfire 3 was one edition,

when they reached Wildfire 5 the name was changed to Creo 1.

Therefore I am quite certain that this forum is the right one.

[Kotom-Eng]

If the question is for Creo or Wildfire or Proengineer, then this forum is the wrong one.

PTC has two CAD systems:    Creo+ and Creo Parametric    and     Creo Elements Direct.

Which makes it confusing.

More, for Creo Elements Direct:

- The 3D software name is Modeling, and

- The 2D software name is Drafting.

For Creo+ and Creo Parametric, use only this tab:

[aputman]

Watch these 2 videos and see if this is useful.  Leo makes mention of curve length at the end of part two but doesn't explain how to do it. 

Part 1

https://www.youtube.com/watch?v=w3sy8NiEpgs&ab_channel=ECognition

Part 2

https://www.youtube.com/watch?v=IaxFUwNWayo&ab_channel=ECognition

[tbraxton]

The length of the hoses in these videos is not controlled explicitly in the sketch. It is done via the flexible component functionality. The OP is asking how to control the length in the sketch. @Chris3 has provided the key functionality to do this in sketch mode.

Create a perimeter dimension in the sketch for all entities and designate a variable dimension in the sketch that will update while the perimeter dim is held constant. You can see an example of the perimeter dimension in use in this recent thread: Re: CABLEVEYOR Mechanism - PTC Community

Watch the video I posted there.

[aputman]

I understand what the OP was asking for.  As I stated, in part 2 of the video, Leo mentions hose length can be controlled thru parameter but he didn't explain how to do it.  The videos I posted were not meant to address the exact issue in the OP, but instead to give some ideas how to model the hoses to be flexible. 

[Chris3]

You want to control your sketch entities with a perimeter dimension:

https://youtu.be/Zig2lhj24WI?t=1097 

[tbraxton]

If you want to lock the length of the "flexible hose" then apply the arc length dimension in the sketch as shown here and lock it.

To add the arc-length dimension, click one end of the arc, then click the other end, then click on the middle of the arc, then finally middle click outside of the arc and you'll get a dimension. Note the "eyebrow" symbol above the arc length dimension below.

[BertilRogmark · Accepted solution]

Many thanks to all of you!

The solution was to (in sketcher mode) convert the angle dimension to perimeter and add a relation locking this perimeter dim to a fixed value.

I had already tried this in part mode but there it was not possible to use the perimeter drawing in a relation – never mind why.

I might add that I am working in 1 plane only, the reason being that the hydraulik hose manufacturer recommends avoiding any twist of the hose.

Thanks again.

My issue is solved!

Bertil

[vnamboodheri]

Hello @BertilRogmark, 

It looks like you have some responses from some community members. If any of these replies helped you solve your question please mark the appropriate reply as the Accepted Solution. 

Of course, if you have more to share on your issue, please let the Community know so other community members can continue to help you.

Thanks,
Community Moderation Team.