Sheet Metal Assistance

[Anonymous]

Can anyone tell me why when I tell this bend to go TO a point it does not go to the point?

 

[JDMather]

I am a bit perplexed by the image.

Can you use standard modeling tools to "fudge" in what you want and then attach the *.ipt file here?

[Anonymous]

I want the flange to extend TO the point selected. It requires an offset of -0.0299 to get there. Seems odd to me that the TO just doesn't go TO.

[Anonymous]

Mirror also doesn't work with sheet metal parts. BLAH

Part attached

[johnsonshiue]

Hi! The selected point defines the vertical distance the Flange will extend. It will not go side way or any non-vertical direction from the bend. Mirroring sheet metal features can be tricky, particularly with bends. In this case, you will need to turn on Adjust option in Compute method (expand the Mirror dialog). Then you will need to trim the extra bends using Thicken Cut. Please take a look at attached part and let me know if more information is needed.

Many thanks!

[Thomas_Savage]

Hello,

If the mirror doesn't work then split the solid on a plane in the middle of the model.

Then mirror the solid on the same plane you split it on.

Then you wont get an error. Like you do with mirror.

Thomas.

[Anonymous]

I appreciate the tips to get this to work, however these are all workarounds to functions that should just work out of the box. Every time I have to look for some unique way to do things my productivity goes down.

To add more misery to my day. I am trying to add louvers to the back side. I created 1 no problem. Now when I go to pattern the louvers the system tells me to use the optimize feature. When I select that option the pattern fails. When I leave it default I can make 1 column of louvers. I need 3 columns of 42 louvers total. It will let me do 3 columns of 33 not optimized but anything greater than 33 fails. 

Am I doing all of this wrong or something? I have not ran into these problems with SW or SE. It is making my job extremely difficult.

[kelly.young · Accepted solution]

You're on the right track for the sheet metal functions, it just takes a bit of prep and practice. I would recommend starting with your base shape on one sketch to Face rather than Face then Cuts. It makes things easier in the long run to change and modify, also less commands. If you know the part is going to be symmetric building half of it will make it easier to make changes and then Mirror, also eliminating commands. Your first Flange can be multiple edges, if they are all going to the same depth it creates continuous corners and gaps. You can edit the bend relief info in the attached screen shot. For the pattern at 42 it prompts it will result in a large number of occurrences, click OK, it should pattern fine just take a while to compute. Check out the updated file, hope this helps.

[Anonymous]

Adding a new default vs using the thickness override solved the problem (again this feels like a bug). The thickness override is somehow causing errors. While I am continuing I have been looking into iFeatures. I drew up a part but I cannot get it to accept both the cutout and the louver. If I select sweep for the louver it doesn't work at all. If I use extrude the save button is grayed out.

[JDMather]

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@Anonymous wrote:

... While I am continuing I have been looking into iFeatures. ....

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The Inventor equivalent of the SolidWorks Forming Tool is a special case of iFeature called Punch Tool.

When creating the Punch Tool you need to be careful about not creating parent/child relationships where the parent will not be going with the Punch (iFeature).  Also, a Punch should have a single Sketch Point in the first sketch of the Punch Feature - this is how Inventor places the Punch.

I notice several other things that I would do differently - I will try to model up an example when I get a chance.

[Hochenauer]

Hi, this is in reply to your original question. As Johnson said, the to input point is a way to measure the height datum. 

The Flange will touch a parallel plane to your new flanges base (red), which will contain your selected point.

I agree the result can be unexpected, but there is value in both the way you expect it to work and the way it is currently working. Please feel free to post to the idea station to get the additional option.

Kind regards,

Gerald

[JDMather]

@Anonymous

Well, I hope you are still around since I just spent a couple of hours working up this example.  2016 example attached.

It is almost always better to pattern a body rather than features (in this case my first body "pattern" is Mirror).

(This principle is true both in SolidWorks and Inventor.)

Drag the End red End of Folded marker to just below Sketch2 and then down step-by-step (this is equivalent of feature roll up bar in SolidWorks).

For the Louvre I used 3 different pattern techniques to demonstrate.

1. First pattern is of the Features.

2. Second pattern is of Sketch Points used to place Punch tool.  In some cases this is the best way to place Punches and is so easy that I use it for non-sheet metal parts too.

3. Third pattern is how I would normally do a Punch pattern in SolidWorks or Inventor (except of course I would do all three rows rather than just one).

I realized that I did make one mistake - but I need to move on to other work.  This example should give you some ideas.

[Anonymous]

This is great. I was working on some other stuff, but now I am back to this. I will review today.

[Anonymous]

So even more fun now. When I go to add the louver to a new part and I need to rotate the louver 270 degrees the feature fails. What is the point of having a feature that is supposed to save time if it does exactly the opposite???? ***BANGS HEAD ON DESK***

**UPDATE**

iFeatures are bound to the original coordinate system which they were designed. If you don't create your next part with the exact same positioning iFeatures will not work. This makes them completely useless. ***BANGS HEAD ON DESK HARDER***

[JDMather]

Attach the geometry you used to create the Punch tool here.

[Anonymous]

I am using the punch tool that you provided in post 12.

[JDMather]

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@Anonymous wrote:

I am using the punch tool that you provided in post 12.

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Oops, I did not take the time to make that a robust tool.

Should be as simple as removing any vertical and horizontal constraints and replace with parallel and perpendicular.

I will try to take a look when I get a chance.

[JDMather]

Try this one.

Rather than banging my head on desk - I used more constructive approach of deleting one horizontal constraint and one vertical constraint and adding one perpendicular constraint.

[Anonymous]

Such a simple modification makes a huge difference