Inventor equivalent, cut normal sheetmetal

[linnmaster]

Hello,

 

For those that are familar with ProEngineer or SolidEdge, they have a feature that's primarily used for sheetmetal which is project/cut normal, or perpindicular, which is essentially a sheetmetal tool used to accurately model the result of a pressed up part from a development which has been processed.

 

I want to get the development of a cutout in a curved sheetmetal part in Inventor so that it's development does not have complex edges. How could this be achieved in Inventor?

 

I will attached a sample file here soon. My Vault is backing up at the moment ...

[JD Mather]

I think what you want is to start a sketch on a planar face of the part and then Project Flat Pattern. Skecth your cut and then Cut Across Bend.

 

In 2010 you can also Unfold/Refold (not to be confused with Flat Pattern or Fold).

[linnmaster]

I think what you want is to start a sketch on a planar face of the part and then Project Flat Pattern. Skecth your cut and then Cut Across Bend.

 

In 2010 you can also Unfold/Refold (not to be confused with Flat Pattern or Fold).

 

I've attached a file of what I would like to cut, but I need the development to give clean edges for NC processing. The sketch geometry is not on a planer face of the part. It's on a user defined plane. I personally find Cut Across Bend not very useful because the result is the same as if I unfold, draw my geometry, cut, and then refold - of course that's a lot more work. Cut Across Bend relies on you knowing the development geometry. I need the reverse, I know the formed geometry, but need the development. Where is Project Flat Pattern if you are using the Classic UI in INV2010?

 

Other issue I have is how to get a cirular hole cutout in the development of the cone, to model in the formed cone. I will attach file shortly.

cutout.zip

[linnmaster]

Cone file attached ...

 

Attempted method will work for cylindrical roll, but not for cone.

 

Next part is getting the sheet metal circular cutout, formed, and assemble into the hole to close it up again. Problem arises as there are no flat surfaces/edges on the circular sheetmetal part to begin with so I can't fold. If I start with contour roll, then unfold, cut out the excess to have my circle remaining, I cannot refold.

conecutout.zip

[JD Mather]

I've got some other work to get to, so I can't post any examples - but one commonly used trick is to model as a surface body, trim as neede and then Thicken quilt. The thicken is going to be uniform thickness will all edges perpendicular to the flat pattern for laser, waterjet or plasma cutting the flat.

[linnmaster]

Hello JD. Thanks for your advice. Problem is that I don't know what the formed sheetmetal part looks like ... ie, the major and minor of the ellipse when the cicular plate is rolled. Hence why I'm having to flatten, cut the circle, and reform. I don't think you can unfold a surface ...

[JD Mather]

I don't think you can unfold a surface ...

 

Thicken. You Thicken the surface by the Thickness paramete and the resulting solid can be unfolded.

[JD Mather]

The real question is, (Is your design intent to have it circular in the flat or have it circular in the folded?" Either method can be done once you figure out a technique.

 

Using trimmed surfaces is a common technique for getting around some problems.

conecutout.zip

[JD Mather]

Here is example with round hole in rolled cone perp to cone.

conecutout perp hole.zip

[JD Mather]

And example of round hole rolled cone perp to cone axis. (of course pull down the EOP in these attachments)

conecutout perp hole to axis.zip

[linnmaster]

The real question is, (Is your design intent to have it circular in the flat or have it circular in the folded?"

 

Hi JD. Thanks so much for your assistance. To answer your question, design intent is to have circular in flat. I tried to recreate a cutout on another quadrant on the same cone using your technique, but have run into a few problems and have a few questions:

1) I'm not quite sure how you created workplane2. Did you use the line in sketch4 and 90deg to xyplane?

2) After creating loftsrf3, and having the loft selected, I cannot seem to trim as it says "cutting tool does not cut any surfaces"? This error seems to be resolved if workplane2 is offset a distance from the cone surface, however, yours works without needing to be offset?

 

My attempt is attached.

 

Kindest regards,

David

DLconecutout.zip

[JD Mather]

Try offsetting the workplane out further for your circle sketch to be projected and wrapped. That way you don't end up with a confusing singularity on the Loft. I was actually kind of surprised that mine worked without offsetting.