Forming Tool for Sheet Metal

[jacek0841]

Can NOT get this working - Help file does not help.

- Do I have a choice to produce my own forming toll ? Like in Indent - or must I use what's in the Library ?

- The forming tool - is it in a separate file or in the part file ?

- give me some simple steps one by one - I am sure it's simple but I am convinced I am missing/misunderstanding some critical steps.

 

[rfus]

Make a folder here (I named mine custom) and put your part in

C:\Program Files\SolidWorks\data\design library\forming tools\custom

You can then access it

 

[rfus]

Of course you still have to use the form tool feature on the part. You can select the stopping face and the faces to remove. Then go put the part in the folder I mentioned above, but note: your design library may have a different path depending on where you installed SW.

RFUS

 

[jacek0841]

... your design library may have a different path depending on where you installed SW.

Simple and understood.

... the stopping face and the faces to remove.

This part I do not understand - could you please explain in simple English what the stopping and what the faces to remove are.

Thanx

 

[rfus]

Make yourself an extruded rectangle and give the bottom of it a stopping face with the form tool feature. Save as test.sldprt. Put this in that directory. Now drag this to your sheet metal part. The stopping face is exactly what it is called, its where the form tool stops and it is used to mate this form tool to the sheet metal. Now edit your form tool and give it a face to remove. This face will be removed from your sheet metal part. Does that explain it.

 

[jistre]

To add to what rfus said, pretend that you've picked your stopping face on your forming tool. Now, imagine that you have a sheet metal surface you wish to use the tool on. The tool is oriented so that the stopping face is parallel to the surface you wish to form. Next, the body of the tool is pressed into the sheet metal, causing the metal to deform around it and the tool is advanced until the stopping face and the sheet metal surface are co-planar. That's what the stopping face does in a a nutshell. It is mated to the sheet metal surface you want to form, and the sheet metal is trimmed around the tool, then reformed to recreate the contours of the tool.

Next, imagine that you've picked a second face on the tool to be a face that is removed. After the forming tool is pressed into the sheet metal and removed, the face of the feature created on the sheet metal that corresponds to the face that is to be removed is deleted from the sheet metal part. Imagine that you had a tool to create a louver. The area of the louver that is open would be a solid part of the forming tool, but by selecting it as a face to remove, it isn't translated to the sheet metal part.

 

[JMirisola]

Don't forget the colors for the faces. I believe it's red to remove, blue (purple?) to indent. Forgive me, I'm color blind...

Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP1.0, Dell M90, Intel 2 Duo Core, 2MB RAM, nVidia 2500M

 

[jacek0841]

.
Thanks folks - I finally got it working - my main error was that I thought the forming tool was to be in the same file, just not merged (multibody), as in Indent case. ...

 

[jacek0841]

.
Next question - after I made the lance I was trying to locally bend it further using icon "sketched bend".

It won't - says: "Failed to make the sketched bend"

Is it not possible or am I doing something wrong ?

 

[CorBlimeyLimey]

You will need to adjust the forming tool sketch.

The Sketch Bend only works on sheet metal and the Lance isn't a true SM feature.

 

[jacek0841]

... the Lance isn't a true SM feature.

What else is not a true SM feature ?

 

[CorBlimeyLimey]

Basically all of the forming tools. They are just solid model features within the SM part. When you hit the Flatten tool, you will notice that the forming tools do not flatten.