Is it possible to make pure wire mesh using inventor

[Anonymous]

Hi, Is it possible to make a pure wire mesh or net structure (without using any graphics texture) in any version of inventor.

If possible, please let me know the procedure.

[mcgyvr]

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@Anonymous wrote:

Hi, Is it possible to make a pure wire mesh or net structure (without using any graphics texture) in any version of inventor.

If possible, please let me know the procedure.

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Sure..  tons of ways..

Easiest..

Sketch a single circle.. extrude.. rectangular pattern to create the one direction members.. then create a new sketch on a plane 90 degrees to that with a circle.. extrude.. rectangular pattern to create the other directional members..

The problem is how taxing that becomes.. Depending on size/complexity it may/will slow inventor to a crawl..

Hence why the graphical texture is the recommended path to take.. There is almost no reason to completely model a net or mesh..

[Anonymous]

Thanks for your reply.
Can you share any video link. I want to make net structure not a grill structure (wire must go in between the other wire, I mean every wire follow a wavy path.)

[mcgyvr]

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@Anonymous wrote:
Thanks for your reply.
Can you share any video link. I want to make net structure not a grill structure (wire must go in between the other wire, I mean every wire follow a wavy path.)

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Before anyone spends the time can you explain why you need to actually model the net structure vs just using a texture?

And in addition to that, can you show an image of exactly what you want..

Using just bunch of "sweeps" vs straight extrusions would allow you to have the "over-under" structure

[Anonymous]

Please go through the attachement.

[ampster40]

if this was flat and not round, I'm sure it could be done. Being that this appears to be in a tube-form, I'm not 100% sure it could be done. But if it can, the modeling needed to produce one wire will be pretty extreme and then multiple that by X number of wires and I can say Inventor will probably cause smoke to come out of your computer. Good Luck.

[JDMather]

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@ampster40 wrote:
... I'm sure it could be done. ....

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I'm quite certain it could be done in Inventor.

(although the image looks like fudged art to me, not a photo of existing mesh part)

[Anonymous]

Thanks for your comment. Please let me know how we can make it, if the feature was flat. It will be better if you share any link or a video.

[Anonymous]

Thanks for your time and effort, But its not a forged part though it seems like. Can you share a link or video for wire mesh creation.

[ampster40]

I've got access to 2014 thru 2016. I will use 2014 to produce an example - but it may be later on today before I can provide a part file.

[ampster40]

This isn't a pretty model by far and it's very simple in that in only includes two wires in one direction and 4 "straight" wires in the other, but it should give you an idea of how to proceed if you choose to. Ref the wire1.ipt file, I failed to take into account the perpendicular wires which would pass thru this single wire shape/profile. Thus the reason for a straight wire, wire2.ipt that you'll see in the assembly. In wire1.ipt, edit or view the "sweep profile" sketch within the Sweep1 feature. When you develop the sweep profile for the first wire, you'll have to take your time and figure out exactly how the perpendicular wires will pass thru this single wire, ie, the center of each arc in the sweep profile will more than likely not be inline or level with the origin or center point as I have modeled - I'd guess the center of each arc of the sweep will probably be offset from center by 1/2 of the wire diameter. The sweep profile sketch I created could be cleaned up a bit/simplified more than I have done. In my example I tend to use construction lines to show the approx. perpendicular profiles of wires passing thru this single wire (just for a visual reference while developing this profile) - so a lot of that construction stuff could probably be omitted or not used. Sorry I don't have a video to link to. I did not search youtube - perhaps someone has already created a video and would show a cleaner way to do this. HTH.

[ampster40]

JD, if you have the time and could model up a "tube" of wire mesh, I would be interested in seeing an example of that.  It's Friday and trying to think how that would work makes my head hurt!  I agree what you said about the pic, the flat profile doesn't seem acurate - considering the top and bottom where the wire mesh rolls around the quadrants.

[JDMather]

A design like this all comes down to a sweep of a 3D intersection path curve.

This tutorial ties a knot.

If you can tie a knot....

The attached tutorial was originally written over 9 yrs ago - there a a couple of changes I might make today.

[Anonymous]

Yeah it can be done using a bunch of sketches with sweep profiles,

but what about

1. If the wire diameter changed !!

2. How you will define the free wire length for that cage/ structure ??

3.If you have to change the in between gaps among the wires !!

[JDMather]

Inventor is a parametric modeler - change simply edit the parameters.

How much experience/training do you have with Inventor?

[Anonymous]

Hi JD & Ampster,

I am very thankful to both of you for your efforts & time. Its really appreciated.

Yeah its a very good parametric software & I am using it form last 4 years.

But if you are going to make all the sketches in circular partten it will be very difficult to handle all its paramenters.

If you have to find that free length of the wire it will difficult, and the total structure to be made in two wires only.

There is also a question about the elongation/ductility property of wire. In sweep command it will not give an exact length.

If you go through that image you can see both the wires are in wavy shape. (cant do it by making one wire wavy & another straight.The structure is almost like a football net.)

I was looking for some special commands or tricky way which can eliminate all those afforts & paramenters.

I have attached an isometric view of a similiar structure (though its not cylindrical).

Thanks again for all your time & efforts.

[JDMather]

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@Anonymous wrote:

If you go through that image you can see both the wires are in wavy shape. (cant do it by making one wire wavy & another straight.....

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I saw the image.  I understood the image.

I see a pattern.

[Anonymous]

Yean it could be done using pattern, but how you will make it in 2 wire. can you share any video link or an inventor file.

[ampster40]

flat wire mesh model done using one wire with multiple patterns. There is a disconnect as well regarding the "profile_count" variable I used, ie, another variable would have to be added in order to translate the profile count into a length that could be used in the assembly. I have to admit the tube model prospect is overwhelming or seems rather difficult still to me at least - even though I can tie a knot! Granted, it might be easy if a single wire will be straight or inline with the quadrant of the tube. I'll keep playing with this. BTW, no mention of what version of Inventor you are using, these models were done in 2016 this time.

[ampster40]

wire mesh tube example (part of) using updated Part1.ipt from previous post (includes a tube diameter parameter now). From this point you would just have to figure out the "round wires" and how they weave in and out of this example. Please note, the angle constraint used for the 2nd wire placed is approx. - that would need further defining thru use of a wire qty parameter which I did not set up in Part1.ipt yet. I'm not too sure I would want to tackle a wire tube model where the wires were not inline with any plane but rather twist around at odd angles.