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How to flatten this form?

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Message 1 of 13
denorm
2056 Views, 12 Replies

How to flatten this form?

Hi,

 

I'm trying to make a template for a six-faceted vase form.  Basically one side of a sweeped hexagon along a curved path which I would like to Flatten in Sheet Metal.

 

First, I have a profile:

 

Fullscreen capture 8292013 103549 AM.jpg

 

Then, I add a hexagonal base sketch:

 

Fullscreen capture 8292013 103600 AM.jpg

 

Next I do a sweep using the profile as a guide rail and the y-axis as the axis:

 

Fullscreen capture 8292013 103625 AM.jpg

 

So far so good.  Finally, I select one of the facets and Thicken to 1mm:

 

Fullscreen capture 8292013 103706 AM.jpg

 

Fullscreen capture 8292013 103725 AM.jpg

 

After converting to Sheet Metal and setting the Sheet Metal default to 1mm, Sheet Metal will not perform a Flatten because it cannot find any bends.

 

Is there any way to go about this in Inventor?  Perhaps using some other method than a Sweep?  Any method that produces a flat pattern would be appreciated!

 

Thanks very much for your time,


Derek

 

12 REPLIES 12
Message 2 of 13
JDMather
in reply to: denorm

Attach your ipt file here. (I am not familiar with editing image files in Inventor)

I posted a very similar example (ipt file) here in the past - a search might turn it up (this would have been 5 or 6 years ago).

 

Is your sketch tangent continuous?

Did you use a spline?

What version of Inventor?

 

Of course none of these follow-up questions would be needed if you had attached your file.


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Message 3 of 13
denorm
in reply to: JDMather

Here is the ipt file.

 

In the past I have had no problems flattening cylinders, cones, and conical sections.  But I am stumped with this type of faceting...

 

Thanks Again,


Derek

Message 4 of 13
denorm
in reply to: denorm

After looking through JDMather's old posts it seems I won't have much luck using a spline.  Unfortunately I could not find the similar example he/she mentioned.

 

I've attached a new, simpler test which uses just a hexagon as a base and an arc (rather than a spline) for the sweep.  The Flat Pattern just gives me a curved surface.  I'm pretty sure this is a developable surface..  (As you can tell I am not an engineer, my apologies..)

 

btw I'm using Inventor Professional 2013

 

Fullscreen capture 8292013 53440 PM.jpg

Message 5 of 13
CCarreiras
in reply to: denorm

Hi!!!

 

Nice Sheet metal exercise!!!

Sometimes for more complex geometry we have to use alternative tools and a little bit of imagination.

I believe there's other ways to create this part... but, you have my version below.

 

 

 

flat_Jar.png

 

Try also the file in attach.

 

It's a little hard to explain all the steps i used, and I believe you will understand looking the file, but if you have questions, go ahead and ask.

 

Regards.

 

solution.png  Did you find this reply helpful ? If so please use the Accept as Solution or  Kudos button below

 



Regards.
CCarreiras
Message 6 of 13
CCarreiras
in reply to: CCarreiras

Hi!

 

Also worked in Inventor 2013.

 

File in attach.

 

 

CarlosC

 

solution.png  Did you find this reply helpful ? If so please use the Accept as Solution or  Kudos button below



Regards.
CCarreiras
Message 7 of 13
denorm
in reply to: CCarreiras

Hi Carlos,

 

This is perfect!

 

In the past when working with simpler items containing cones and cylinders I would simply model the surfaces, thicken, convert to Sheet Metal and rip along the join line.

 

It seems obvious now that for this faceted item that I should have tried Sheet Metal tools as you did.

 

I still need some time to study your work, I have never before used splits and projected loops as you have done.

 

But I understand the basic concept of using Contour Flange..  I will keep studying!

 

Best Regards,


Derek

Message 8 of 13
yannick3
in reply to: denorm

Hi

Here is mine

it keep original spline and all in sheet metal maybe impossible to fold.flatpatvase.JPG

Yannick Verreault
INV PRO 2015
MS Office 2007
Win 7 pro, core i7 950, asus P6T WS
nvidia Gforce GTX 295
WD caviar black 500Go
WD caviar black 1To

Message 9 of 13
CCarreiras
in reply to: denorm

Hi!

 

I use also (and a lot), thickness tool to create complex sheet metal parts. It's a lot better then using loft, sweep or shell.

 

You can use the thickness option when your geometry is based mostly in arcs and lines, that produce cones,etc. I think the program can interpret these arcs like bends, calculating the compensation needed.

 

When our sketch is based in splines, its better to use a Sheet metal tool to create the solid.

 

Pay attention, in my the model, the thickness of the part was pointed to outside the surface, you had this thickness at middle surface, so, maybe you have to do some adjustment.

 

Bye.



Regards.
CCarreiras
Message 10 of 13
denorm
in reply to: CCarreiras

Hi Carlos,

 

I've tried to copy your example every way possible, but I always get stuck at the Unfold.

 

The steps as I undersand them:

 

1.  Use a spline, arc, or other drawing tool to create a profile.  Create another drawing of a hexagon or some other straight-edged form to create the base.  Sweep the base up along the profile to create a surface form.

 

Fullscreen capture 8312013 24721 PM.jpg

 

 

2.  Create a new work plane that intersects perpendicularly to one of the facets of the form.  Create a new sketch on this plane.  Project the geometry of the surface form onto this sketch.

 

 

Fullscreen capture 8312013 24819 PM.jpg

 

3.  The sketch forms the profile for a countour flange created with the Sheet Metal tools.  (Ensure your Sheet Metal defaults are set properly when converting to Sheet Metal.)

 

Fullscreen capture 8312013 24952 PM.jpg

 

4.  Create two new work planes following to vertices of the base hexagon which are adjacent to the line that forms your countour flange.

 

Fullscreen capture 8312013 25040 PM.jpg

 

5.  Create two new splits using the two new work planes and the inner face of your contour flange.

 

Fullscreen capture 8312013 25319 PM.jpg

 

6.  PROBLEM HERE:  Unfold the contour flange.  I have tried this step in many ways but always get one of two errors, either "Could not attache to face: face could not be found." or something like "cannot find any bends to unfold".  However, when I use your ipt file and delete your unfold I can re-unfold with no problem. 

 

Fullscreen capture 8312013 25605 PM.jpg

 

If you could provide any tips I would greatly appreciate it!  My problem ipt file is attached.

 

Thanks!

 

Derek

Message 11 of 13
yannick3
in reply to: denorm

Hi

see attachment R2013

Edit

first the unfold feature need reference plane inherent to the model and the unfold feature it's not the same that flat pattern

Yannick Verreault
INV PRO 2015
MS Office 2007
Win 7 pro, core i7 950, asus P6T WS
nvidia Gforce GTX 295
WD caviar black 500Go
WD caviar black 1To

Message 12 of 13
denorm
in reply to: yannick3

Wow!  Thanks Yannick!  In the end your solution was very simple and elegant.

 

Now I can use my normal process of modelling surfaces, then thickening, then flattening.  The most important thing I learned is "reference plane inherent to the model".

 

Thanks again to you and Carlos for taking time to help me.  I am just a craftsperson and sometimes Inventor can be quite difficult for me, but I learned a lot this time.

 

Best Regards,

 

Derek

 

 

Step 1.  Model a faceted form (cylinder, sphere, beach ball, vase, etc.) using a profile spline and a base polygon.

 

Fullscreen capture 8312013 24721 PM.jpg

 

 

Step 2.  Create a 2d sketch on the YZ plane.  Project the cut edges of the form.

 

Fullscreen capture 912013 91618 AM.jpg

 

 

Step 3.  Create two new work planes using the form's Y axis and offset from the YZ plane by x degrees.

 

Fullscreen capture 912013 91701 AM.jpg

 

 

Step 4.  Create a surface extrusion between the two planes using the sketch from Step 2.

 

Fullscreen capture 912013 91801 AM.jpg

 

 

Step 5. Thicken the new surface.

 

Fullscreen capture 912013 91830 AM.jpg

 

 

Step 6.  Convert to Sheet Metal, remembering to set the Sheet Metal defaults appropriately.  Go to Flat Pattern to see the final template for the thickened facet.

 

Fullscreen capture 912013 91907 AM.jpg

Message 13 of 13
CCarreiras
in reply to: yannick3

Hi!!

 

There's no problem about the way your trying to unfold. There is no  solution to unfold the file. Somethimes Inventor likes to go one way, and somethimes like to go other way, maybe if you do the sketch in another plane, maybe itr

starts to works ( it's math!!!  Smiley Happy   ).

The important thing is:  its better to know several processes to achieve the same result, mainly in sheet metal... and in this case you had learned two different aproaches for the same part!!

 

Regards!!



Regards.
CCarreiras

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