Extruded threaded hole? 1

[spaneard]

Hello,

I've recently started trying to learn this fine program SW2007 for my work, where we are oft in need of simple L brackets to support computer parts inside various chassis.

There is a specific type of threaded hole that I've seen on sheet metal, and my metal shop tells me its called an extruded hole.

This adds threads and needs no pemnuts or other inserts, but rather extrudes the metal.

So my question is in three parts.

Is there such a feature in solidworks? If not, why not? If yes, what are the steps to add such holes?

Secondly, does this process bend the metal and thus alter dimensions of the whole assembly? Or do I not need to worry about that.

Third, if the feature does not exist in SW, is it simply a matter of adding comments on the drawing to make such and such hole an extruded thread, give thread details and in what direction to extrude?

Thanks for any help.

-Henry

 

[CorBlimeyLimey]

Answer - First part;
Yes. An Extruded Hole feature is in the Design Library > forming tools > embosses section. If this is the first time you have used the forming tools, you will have to RMB on the folder and select the Forming Tools Folder option before using any of its features.
A Cosmetic Thread will have to be added manually.

Answer - Second part;
Yes, it bends the metal, but does not alter the overall dims in the model. If the part is very small, dimensions may be affected in the actual part.
NOTE: When the part is shown in its flattened state, library features will NOT be flattened.

Answer - Third part;
Sheet metal features can easily be created and added to the library. Check the Help file for details.

 

[MadMango]

The process as I know it is called Flowdrilling. Please see

http://www.flowdrill.nl/

to ensure we are talking the same thing.

If this is something that you are going to be using a lot of, I suggest creating a Library feature that you can use repeatedly in the future. Modeling it accurately may not be an automatic thing, and you may have to create a sketch profile and Revolve the feature.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[CorBlimeyLimey]

Oooh, right. I had forgotten about that one. A

for the reminder.

 

[spaneard]

Thanks Corby, Mango.

I'll take a look at the forming tools later today.

I took a look at the flowdrill process and it does not seem to be what I'm refering to, but I could be wrong. So just in case you were both talking about the same but different thing, here's a picture of what I mean. You can see one side stays flush, unlike the flowdrill process which appears to need finishing after the tapping is done.

-Henry

 

[CorBlimeyLimey]

The image you show is similar to the SW extruded hole feature, but SW does not include the thread form. The threads were probably added by a separate process.

 

[ctopher]

It looks like a type of PEM nut.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)
ctopher's blog

 

[smcadman]

It is a 2-step process, sometimes 3 if you need to elongate it further. First the flange is created in a punch then it is tapped.

Solidworks already includes the round flange for sheet metal, but if you can't find it use this one. Put this in the Extruded Flanges folder in your Forming Tools folder. Copy this tool and modify it as required then drag-n-drop it on a sheet metal part.

http://www.paul-flores.com/downloads/round_flange.sldprt

Flores

 

[spaneard]

Hello,

I managed to figure this out with all of your suggestions. Using the round flange forming tool.

The more I think about it the more it seems this tool is not making changes I can reliably measure, or its not meant to.

I modified the forming tool into a 3mm dia for an M3 tapped hole I need here for starters. I made the outer diameter of the flange some random diameter bigger than the 3mm hole. No idea if I should care about that at thit point.

Some questions on this and the cosmetic threads:

1) When dealing with a sheet metal supplier, does the fillet bend radius of the forming tool matter. Should I be requesting any data from them to form these holes properly? SW only tells me the bend should be less than the thickenss of the sheet metal.

1a) The forming tool has the cutting portion, which is a cylinder of 3mm diameter and some length past the fillet bend. Do I need to adjust this length in any way to accurately protrude the metal? Does SW calculate some real physics here?

1b) Can I now tap this formed hole in any way? Corb mentioned I will need to do cosmetic threads, which will take me to question 2. But is this a hole I can TAP in SW?

2) Cant seem to make cosmetic threads on formed objects. I can create them on standard tapped holes, but not on the 3M hole above that I formed.

Excuse the noob questions.

Thanks,

-Henry

 

[rollupswx]

...3mm dia for an M3 tapped hole

The hole size for an M3 tapped hole is not 3mm.

 

[CorBlimeyLimey]

Firstly, if you are creating a hole for a standard M3 thread, the inner dia should be Ø2.5mm. The outer dia will be determined by the material thickness being formed.

1) Many standard size forming tools exist. Either have your SM supplier obtain a tool suitable for your needs, or you contact the tool suppliers direct for the info you need.
The minimum radius of the forming tool should be greater than the material thickness. This allows an inside radius to exist at the underside of the formed material.

1a) SW does not calculate the protruding length. That is a function of the tool created and knowledge of the formability of the material being formed.

1b) Yes.

2) Select the inner protruded edge of the formed hole when applying the Cosmetic Thread.