Punch Direction Issue

[arkelec]

I can't work out what's wrong with the attached punch file. 

It will only orientate in one direction.

I've (tried to) follow this thread https://forums.autodesk.com/t5/inventor-forum/punch-feature/td-p/4829671 (where @JDMather gave some useful tips) & also this one https://forums.autodesk.com/t5/inventor-ideas/extruded-holes-for-metal-sheets/idi-p/6915028

As far as I know, I have not used any projected geometry, but I have no idea what the issue actually is.

Could someone take a look & point to my errors.  Thanks in advance.

PS: I tried to attached the ide file, but verboten. 

[JDMather]

Change the Solid Sketch to 100x100

Drag the Cut-out sketch well away from it's current location.  What do you observe?

Now, Edit the Profile Sketch.  What do you observe?

Also, what is the correct tap-drill size for a M5 thread?

If you drill a Ø5mm hole and place a M5 fastener into the hole - what behavior will you observe?

[arkelec]

Thanks for the quick response.

Change the Solid Sketch to 100x100 - Done

Drag the Cut-out sketch well away from it's current location.  What do you observe? Rotate constrained to Y Axis

Now, Edit the Profile Sketch.  What do you observe?  A mess

Also, what is the correct tap-drill size for a M5 thread? 4.2mm 

If you drill a Ø5mm hole and place a M5 fastener into the hole - what behavior will you observe? Got it.

I think I fixed everything, but still the direction is the wrong way.  What else am I missing?

[JDMather]

Edit the Cut-Out sketch and drag the circle on the screen.

You should be able to drag it anywhere without unexpected behavior (the two construction lines should stay through the center of the circle).

[JDMather]

Edit Profile sketch.

Click and drag one end of the line used for axis of revolution.

It should have a Parallel or Perpendicular constraint so that it maintains correct orientation.  I would go ahead and fully define the sketch.

[arkelec]

Yeah, I noticed one of lines was adrift, it does have a perpendicular constraint to the first one but I've added a dimension constraint.

The cut sketch & feature now moves around intact.

But it still doesn't work.

I assume I've made the correct selection:

[arkelec]

I've been on this for 3 days now, if some kind soul could put me out of my misery, I'd appreciate it.

[arkelec · Accepted solution]

Sooooo, after another stab at this, I finally worked out what was wrong (it might help others who are struggling):

1. Some local dependencies (horizontal and vertical constraints) still present, as mentioned by @johnsonshiue in post 23 on this thread https://forums.autodesk.com/t5/inventor-forum/punch-feature/m-p/7094195/highlight/true#M644130 - F8 shows the offending items 
2. Only project a single geometry as per the instructions from @JDMather step 4 of post 7 [https://forums.autodesk.com/t5/inventor-forum/punch-feature/m-p/4830411/highlight/true#M498263] 
3. When constructing the profile sketch, delete any horizontal and vertical constraints & apply Parallel, Perpendicular or Equal constraints.

What a way to spend a weekend!

[johnsonshiue]

Hi! I think this behavior has been discussed before. Indeed, iFeature (Punchtool) does not allow the user to specify the exact axial direction (0 or 180 deg). This can lead to undetermined direction.

For your case, you may consider using Extrude instead (with fillet in the back), since its direction is persistent relative to the sketch plane.

Many thanks!