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:
Then, I add a hexagonal base sketch:
Next I do a sweep using the profile as a guide rail and the y-axis as the axis:
So far so good. Finally, I select one of the facets and Thicken to 1mm:
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
Solved! Go to Solution.
Solved by yannick3. Go to Solution.
Solved by CCarreiras. Go to Solution.
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.
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
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
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.
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.
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Hi!
Also worked in Inventor 2013.
File in attach.
CarlosC
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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
Hi
Here is mine
it keep original spline and all in sheet metal maybe impossible to fold.
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.
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.
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.
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.)
4. Create two new work planes following to vertices of the base hexagon which are adjacent to the line that forms your countour flange.
5. Create two new splits using the two new work planes and the inner face of your contour flange.
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.
If you could provide any tips I would greatly appreciate it! My problem ipt file is attached.
Thanks!
Derek
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
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.
Step 2. Create a 2d sketch on the YZ plane. Project the cut edges of the form.
Step 3. Create two new work planes using the form's Y axis and offset from the YZ plane by x degrees.
Step 4. Create a surface extrusion between the two planes using the sketch from Step 2.
Step 5. Thicken the new surface.
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.
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!!! ).
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!!