Single Line Cuts using Laser

[ClintWestwood]

I am working on a project where several holes in a sheet metal part will need to be cut as "knockouts". In previous years, either an engineer or the laser cutter programmer would set up the machine to partially cut a circle, but leave a gap to hold the knockout in place (basically a 340 degree arc).

Now that we are using Inventor, is there a way that we can create these features so that they show up in a dwg as a single line? It must be a single line; some of the holes are very small and if the laser makes more than one pass it could affect the integrity of the feature.

The closest I have gotten to accomplishing this is a surface extrusion on the folded part. When I send it to an .idw file, the line appears in the folded model, but I need it to appear in the flat pattern. I am attaching a simplified example to this post to help explain what I mean.

[-niels-]

If you right-click on the sketch of that surface extrusion and select "copy to flat-pattern", does that give satisfactory results when sent to the laser cutter?
(it copies the entire sketch, construction lines and all.)

[mcgyvr]

I believe it should be done with a "punch" tool in Inventor that has a "simplfied representation" sketch.

I tried to find some help/tutorials on that for you but can't.. 

But I suspect its as easy as creating an extra sketch to select with your single arc during ide creation.

[ClintWestwood]

I copied the sketch to the flat pattern like you said, but the sketch on its own does not appear in a idw or dwg.

I tried to create the surface extrusion on the flat pattern's sketch as well, but the option to change an extrusion to a surface extrusion is grayed out in the flat pattern environment.

[andrewiv · Accepted solution]

Here is a quick punch tool that would accomplish what you want and your original part using this tool.  On the flat pattern you have to use a simplified representation of the punch to get the single line.

[karthur1]

How about using the "New to 2014" Slot tool to draw a slot. Makes that really easy to sketch.  Make the width of the slot less than the kerf of the laser.  Not sure if the laser software will try to cut around the perimeter of the slot of not.

Then do an extrude cut.... that will show up in the flat pattern.

Kirk

[karthur1]

---

@ClintWestwood wrote:
I copied the sketch to the flat pattern like you said, but the sketch on its own does not appear in a idw or dwg.

I tried to create the surface extrusion on the flat pattern's sketch as well, but the option to change an extrusion to a surface extrusion is grayed out in the flat pattern environment.

---

After you copy the sketch to the flat pattern, there is no need to make the extrude surface.  You can include the sketch by right clicking on the flat pattern in the idw browser and then "Get model Sketches".  You will have to manually hide the lines that defines the angle.

Kirk

[-niels-]

---

@karthur1 wrote:

---

@ClintWestwood wrote:
I copied the sketch to the flat pattern like you said, but the sketch on its own does not appear in a idw or dwg.

I tried to create the surface extrusion on the flat pattern's sketch as well, but the option to change an extrusion to a surface extrusion is grayed out in the flat pattern environment.

---

After you copy the sketch to the flat pattern, there is no need to make the extrude surface.  You can include the sketch by right clicking on the flat pattern in the idw browser and then "Get model Sketches".  You will have to manually hide the lines that defines the angle.

Kirk

---

You're right when it comes to showing it on an .idw, but i'm guessing he's exporting to .dxf to get it to the laser cutter.

I tried it myself and he's right, the sketch won't show up in the dxf.

The solution posted with the punch tool with simplified representation does work though.

And you could even set that up so the folded model would get an actual (full) hole, but the flat pattern shows only the simplified version.

So i'd say that that's probably the best way to handle this.

[ClintWestwood]

andrewiv's punch tool seems to have done the trick, thanks for everyone's help on this issue.

[ClintWestwood]

andrewiv, How did you create your punch tool? I am trying to create a slightly different punch for a different set of holes, and the punches I am making keep producing multiple lines in my dwg as opposed to the single line which came out of your punch.

I tried to edit the punch you created, but I am having trouble with it.

[andrewiv]

Start a new part and create the feature along with another sketch that represents the simplified punch.  Then in the Manage tab use the extract iFeature command to create the ide file.  Here is the dummy part that I used to create the iFeature.

[ClintWestwood]

Could you please explain how the simplified punch/simplified representation works? I am self-taught in punch creation and have not needed to know how to use them in the past. I'm able to edit your dummy part, export the ifeature, and apply it to a new part. My dwg is still showing the whole punch.

I'm assuming there is a way to have the dwg show only the other "sketch that represents the simplified punch"?

[andrewiv]

Two things.  First, When you extract the iFeature you have to choose the sheet metal punch ifeature type.  Then select the extra sketch as the simplified representation of the punch.  Next when you create your flat pattern you have to choose how the punches show up.  Go into edit the flat pattern and on the punch representation tab you can select 2D sketch representation.

[ClintWestwood]

That worked, thanks! I hadn't done the second step.