Using a sheet metal punch as pattern feature

[Tranquill]

Hi all,

I searched for this a long time and I couldn't find a solution so I guess it's not possible but I'm not giving up without asking the guru's here.

We make a lot of metal plates with inserts, a lot of the same items are used so we created a few punches which are great.

In almost all cases PEM's are inserted in the holes, but we cant seems to use the "feature pattern" on the punch, is there something we are missing here.

Or can we add something to the punches which makes it possible?

Or are there better ways of going about this?

All tiptricks/info are welcome!!

I'll add a picture for clarity. (I hope)

Pattern

Kind regards,

Aram.

[johnsonshiue]

Hi! It should work unless there is missing geometric condition in the punch. But, if it was the case, you would not be able to insert the punch tool to begin with. Something is wrong. Could you share an example here? I would like to understand the behavior better.

Many thanks!

[TheCADWhisperer]

Are you using sketch pattern of sketch points to place the Punch Features?

Or are you using one Punch Feature and then Feature Pattern?

Are you then attempting to use Component Pattern to follow Feature Pattern (not sketch pattern) for the PEMs in Assembly?

Is this Inventor 2019 or is it with older release?

[Tom_Sturtevant]

Hi Tranquill,

If your punch includes the rectangular cut and the pattern of holes then AFAIK you are out of luck.  Feature patterns that are internal to a punch are not available to Pattern Component.

As TheCADWhisperer said, creating a single hole (either as a Hole feature, a Cut, or a simple Punch) and then creating a feature pattern of the hole will allow you to create an associative component pattern in the assembly.  If you do go that route the “Sketch Driven Pattern” is probably the simplest way to define the occurrence positioning.

Thanks,

T.0.M.

[Tom_Sturtevant]

Hi Tranquill –

Well, you said “All tiptricks/info are welcome” so I’ll share one awkward workflow (“work-around-flow” maybe??) .

The overview of this workflow is that you place your punchtool with the internal pattern of holes, then you create a pattern of Workpoints coincident with the holes and make your component pattern associative with the Workpoint pattern…  Here are detailed steps.

1. Place the punch

2. Create a sketch, project all the punch holes, (window) select the centers and convert to Center Point.  Exit sketch.

3. Place a Workpoint on one of the sketch center points.  Create a Sketch Driven Pattern, select the Workpoint.  Turn off visibility of the workpoints.

4. In the assembly SWITCH TO MODELING VIEW in the browser (only way to select the pattern of Workpoints).  Component pattern, select the Sketch Driven Pattern in the browser.

5. Bam.

Maybe that helps...

T.0.M.

[Tranquill]

Hi, thanks for your reply,

Which file would be helpfull, just the sheet metal plate with the punch in it?

I attached such a file, if you need more please let me know. 🙂

Kind regards,

Aram.

[TheCADWhisperer]

Place ipt file and the punch ide file into a folder.

Right click on the folder and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file here.

[Tranquill]

Ok, let's see if this works, I never uploaded a file here before. 🙂

Here goes nothing..

Aram.