To show the properties of each component in my BOM

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1

Good evening

In the end I would like to show the length properties of each body that makes up my piece (Bar of 80) in the nomenclature (The length of the gate varies so the number of bars too, the length properties of each bar should appear in the nomenclature by just changing the length of the gate).

I think that we should not create the part as I did it (see attachment), because I have only one part so I can't make all the bodies appear in the nomenclature.

Another method that I tried but that also didn't work was to make a piece (bar of 80) that I repeated X times and I did a removal of material on all the parts. But the problem was that in the nomenclature we only saw one part (bar of 80) but with the quantity equal to the number of bars, it did not take into account the removal of material.

If anyone has an idea to propose to me, it would help me bcp.

Thanks in advance!


test_pour_propriete_longueur.zip
2

Hello

 

For this kind of project, I advise you to work with the mechanic welding module.

 

Make your gate with welded parts and then in your drawing, insert a list of welded parts.

 

When making a change, it will be enough to update the list of welded parts by right-clicking on it and pressing "update"

 

See image for details.

 

 

 

 


1.png
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3

Thank you for your answer Bart but I would like to have some clarification on one thing.

I agree to make the bars with the mechanically welded module (I can modify directly  in the assembly the rod part so that it becomes a mechanically welded part). 

My main concern is that ideally I would like to be able to make only one part with its length property and to be able to duplicate the extrusion function to the body with its length property that would change automatically.

I don't know if it's very clear but is it possible to repeat an extrusion function to the body (because my Length property is defined in the equation with the measure tool where I take the edge as a reference) and the length property of the new body calculates automatically.

I don't know if I have the right method but in the end I would like to create only a length property

on one element and that it automatically calculates on the other elements.

Thank you in advance.

4

@Bart's response is very good

It's up to you to realize via the welding mechanic to have via your profile library

all the elements as well as the lengths and cuts if they are worth

so you will have a complete and well-defined nomenclature

See this tutorial among others

https://www.youtube.com/watch?v=ZedPlephfZ4

everything is there, just follow

@+ ;-))

5

continuation of the message in PM

See this tutorial

http://www.leguide3d.com/profiles/blogs/param-trer-une-pi-ce-avec-des-quations

@+ ;-))

6

"Duplicate the extrusion function to the body with its length property that would change automatically."

 

It is this passage that I do not understand.

 

Do you want a video showing you the principle?

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7

Good evening

I still have a small problem with this gate that varies in length.

I attach 2 solidworks files that I made, it's simply 2 different examples.

In fact I would like to have a mix of the 2. That is to say that the demo test file is good for the drawing with the properties (That's exactly what I need in the end) but on the other hand where it doesn't suit me is when I want to change the length of the portal in the assembly (Skeleton sketch), I am forced to re-add bars and/or modify the material removal function.

As far as the demo 2 test file is concerned, the problem is in the drawing or the I don't have the properties because in my assembly the bars are not made with the mechanically welded element function. But on the other hand in the operation of the assembly for me it's perfect (Except that as the bars are not made with the mechanically welded element function it doesn't work in the drawing).

In the end, I would like to have the drawing of the demo test file and the operation of the assembly of the demo test file 2. 

I don't know if it's very clear but I think that looking at the solidworks files it should be easier to understand what I would like.

PS: these are not assemblies but 2 parts files with their drawing.

Thank you in advance for your help. 


fichier_de_demo.zip
8

Looking at your files, I don't think that's the right way to do it.

 

If I understand correctly, you have 3 problems:

- The configuration of your bars so that they are calculated according to the length of the gate.

- The removal of material that you do to adjust your tubes.

- Your Welded Parts List that does not update when changing sides.

 

To set up your rungs, you need to enter an equation in your sketch so that the number of rungs changes according to your length. (Example: Number=Lg/o.c.)

For material removal, there is an Adjust/Extend function in the mechanical welding module that allows you to do what you want to do with your material removal.

And for the parts list in your drawing, if you've followed all of these guidelines, your table should follow.

 

Overall, you can simplify your design.

I saw that you had made a function by elements, naming them by their locations. (Upright, crossbar etc...)

I advise you to group all the identical profiles in the same function, via the "new group" function. (All 50x50 tubes together etc.)

Then, on your drawing, you will only have to insert bubbles to recognize your pieces.

 

I am attaching a simple example.

 

 

 

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9

The problem is not the number of bars because in my sketch I have the right equation which means that if I change the length of the gate the number of sketches of bars is modified (But since I have to use the mechanically welded element function, I am obliged to have the mechanically welded element function of the bar edited to be able to add according to the number of sketch appeared for the bars). In fact I would like to repeat the function of the mechanically welded element of the bar but it seems to me that we can't. In fact, I would like to be able to change the length of the gate and that my mechanically welded element function create the bars according to my sketch which will have been updated automatically (Because the sketch is good, if I change the length I have the sketch lines corresponding to the number of bars).
Kind regards

10

Trying to give you an example, I realize that it's a little more complicated than that and I understand your concern better.

 

There are two problems:

 

- The fact of having a high arched crossmember. So your sketch of the bars must protrude above this crossbar (because the sketch adjustment cannot be repeated.). This forces us to remove bodies that are above.

- The number of adjustable rungs. Since you can't tell Soldiworks to modify the function to add rungs according to the length, it also freezes.

 

I think that if you really want to set up a portal to add or remove rungs according to length, apart from creating configurations of several central rungs, I don't see any other solution.

 

I'm doing the test tonight and sending you the result;)

11

Here is the result.

 

For me, if you want to make a configurable portal, you will have to make configurations.

 

As many configurations as there are different rungs.

Then, link each config to each corresponding function.

 

Try on my part, click on the "8 rungs" configuration and then on the "10 rungs" configuration.

 

 


portail_parametrable.sldprt
12

Thank you for all the answers,
So I looked at your file and I think it could take a long time to do all the configurations. especially since I don't know in advance all the lengths of gates.
So I think I'll make a portal with a very long length (Length that won't be feasible because it's too big) and I'd duplicate this drawing to make the requested lengths (So I wouldn't have to add a bar).

Thank you again for all these answers,
Good luck and happy end of year celebration.

Kind regards

13

That's what I tried to do.

 

I did a test on a 12 meter gate but when changing sides, the function is wrong....

 

I advise you to make several gates, one from 1m to 1m50, another from 2m to 2m50 etc....

14

Hi all

A very simple solution: start with the bars and remove material from all the bodies of these bars, then continue with the rest of the bodies and that's it.

See attached file in SW2014.

@+

Edit: with a repetition of course

 


essai_demo_coyote.sldprt
1 Like