Modelling my inboard-suspension Haynes chassis in Solidworks and have come across a peculiar problem:

I've got some round tubes in it. The profile of the tube is 19mm OD, 2mm thickness (17mm OD).

When I go to "unwrap" the tubes the flattened pattern is ~56.558mm wide, which equates to exactly 18mm diameter (when times by Pi).

Can anybody tell me what I'm doing wrong, all do i have to do all tubes with effectively nil-wall thickness in the profile?

I'd rather avoid that as this way (using realistic profiles) I can keep a realistic chassis mass estimate going.


Any help is much appreciated!

Ta,

Pavs

Firstly, why are you unwrapping round tubes? I can't see any need to do that operation.
But as for why you modelled it at 17mm but the 'unwrapped' dimension appears more, I believe its to do with bend allowances and K values of materials. For example, a bit of steel angle 50mm by 50mm when flattened will not be 100mm. Solidworks is allowing for this difference in the way its flattening it. You can tweak the band values, but from my experience (I often model pressings and develop the flat pattern for laser work) the SW standard figures are pretty close to real world figures.

19mm, 2mm wall tube is 15mm ID

secondly, why would you want to unwrap them? i assume it takes it as a centreline for the sheet profile, so the mid circumference of 19mm 1mm wall tube is 18mm since the inner is compressed and the outer stretched.

why can't you model it as a tube? you'd get accurate data then

Apologies, I should clarify:

Yes, you're right, it's not 2mm it's 1mm (19mm OD 17mm ID)

The chassis is built up of weldment tubes (not wrapped etc.)

However, where there are complicated round tube interfaces, in order to obtain a cutting template for the end profile, I do as follows:

- Select tube
- Insert as new part
- Insert plane across the middle
- Make a 0.001mm slit in it
- Insert Bend
- Flatten bends

This gives me a cutting template which I can print out and wrap around a tube to make notches on the ends..

I just can't understand why it uses an effective diameter of 18mm.. I guess it just takes the centrepoint as you said? In which case there's no alternative but to set a negligible wall thickness for the profile before unwrapping.

Could you just use the Tube Mitre program?

No, because I've got things like nodes where several tubes (and square box section) come together. Like I said, unwrapping it isn't the problem, it's the fact that it takes the centreline between the OD and the ID, and I'm wondering whether there's any way to unwrap it going by the OD surface.

Thanks all

I've had a word with our Solidworks gurus this morning and they said:

quote:

---

Right click on 'Sheet metal' in the parts list (left column)
Edit feature
In the bend allowance box, you need to twiddle the K factor, bend allowance and bend deduction. This will let you put the bend onto the outer face which is what you need. The default is for Solidworks to put the bend on the median.

---

Excellent, thanks!! I'm on SW 2009 too.

I'll have a play around with it (I know where the parameters are located, just never needed to twiddle them before).


Cheers again

Didn't someone post that as the first reply...... oh yeah, me

haha sorry, when you said band values it just went straight over my head, whereas I recognised seeing K-factor in the properties (just never previously touched it).

Both of you can give yourself well deserved pats on your backs!

Success!

For those of you that are wondering, just set:

K-Factor = 1 (as standard it's 0.5 which is the midpoint)

unwraps the OD beautifully now. None of this messing around with infinitely thin tube profiles!


THanks again chaps