Working out the length of part extruded to point

[dvenn42]

Hi,

I'm creating an assembly of tray and trunking routes and my client wants the drawing bom to identify the total length of tray runs. This isn't a problem when creating tray extruded to a given length (and changing the bom setting within the part), however if I create the part within the assembly and extrude the sketch to a point I cant find the length detailed anywhere for the extrusion to transpose into the bom.

Any ideas will be greatly appreciated.

[CGBenner]

@dvenn42 

Hello and welcome to the Community!

Can you please share some images, or an example of what you are trying to accomplish?  From the description alone, it will be hard for people to give you the best advice.  It is also a good idea to mention the version of Inventor, since tools do sometimes change and the solution may be different.  Thank you and good luck!

[dvenn42]

Hi Chris, Thanks for your reply, please see below for clarification on what I'm trying to achieve.

I've started creating an assembly within Inventor 2019 in which I've placed various trunking components that I have modelled, I'm now modelling a new part (Trunking) within the assembly using one of the existing parts as a sketch plane. I'm then extruding the sketch to  a point on the next component rather than extruding to a distance to join these components. Extruding to a point is easier as all the components have been placed within the assembly constrained to a skeleton model.

We're probably using the incorrect software package to achieve our goal, but it's what I have to work with.

I've attached a file, I hope it makes sense.

Many Thanks.

[tomasz.sztejka · Accepted solution]

If not totally 100% accurate answer is sufficient for You then You may try to deduce the length from the crossection area of extruded shape and a total volume of extruded solid:

Volume = Crossection_area x length_of_extrusion

You may attach an iLogic to each geometry change of that solid and update the parameter of a part.

Below is an example I used to compute the length of adaptive cable:
'
' Computes length of cable from it's volume and known parameters.
'
Dim volume As Double
volume = iProperties.Volume() <-- asks current part colume
' This retrives volume, but in "document unit"
L_param= (volume )* 4 / (3.14 * Dia*Dia) <-- L_param is an f(x) parameter to update
                                      ^--- this expression is basically an area of crossection. Supply it with proper constant.

[dvenn42]

Many Thanks for your reply Tomasz,

I'll have a look at this but, I guess this would mean I'd have to create an ilogic for each piece of tray I've created (latest count 140+).

I'd have thought somewhere within the part that's been extruded (to a point) it would have the length parameter that I'd just be able to grab, but parameter "D0" is embedded in the extrusion. Is there a way of just extracting it?

Thanks

D

[tomasz.sztejka]

Dimension which are not adaptive should be visible in f(x) Parameters table in part. They should be visible on drawings in texts under "Model Parameters" ( I know there are some limitations to that tough). 

Dimensions which are computed through an adaptive process are not visible, as far as I know, but You may extract them by making a sketch and placing a driven dimension on it. Then the driven dimension will appear in f(x) table and will be possible to extract and put on drawing.

Alternatively You can create numerous 2D sketches in assembly, project edges of Your elements and insert driven dimensions there. They will be then available at f(x) Parameters table in an assembly.

One way to another there I can see no easy way to extract those lengths if You did not prepare for it from the beginning.