topic Re: iFeature extracting problem in Inventor Forum

iFeature extracting problem

Anonymous — Thu, 12 Apr 2018 18:18:44 GMT

I have just started playing around with the Ifeature command. I would like to create an Ifeature for my sheetmetal feature. I am aware that I cannot have any geometry that is linked to anything other than the feature. Everytime I try to extract the Ifeature I get the following error

"The sketch does not qualify as a punch placement sketch. A punch placement sketch can only have one center mark".

So I looked at my sketches and cannot see more than one centerpoint, unless it is trying to use the center point of two small relief radii.

Using Ifeatures

Anonymous — Thu, 12 Apr 2018 19:16:09 GMT

I have created an Ifeature (which is attached). When I try to adjust the size, it fails?

Re: iFeature extracting problem

jhackney1972 — Thu, 12 Apr 2018 19:23:18 GMT

I do not see a problem with your sketch as far as center points. I did delete two workplanes that were not doing anything before I created your sheet metal punch. Your question talks about creating an iFeature but the body of your question, and you model, suggest you are trying to create a sheet metal punch. That is what i did. Please see the screencast. Inventor 2018 model is attached.

Re: iFeature extracting problem

Anonymous — Thu, 12 Apr 2018 19:29:56 GMT

Thanks for the speedy response. Part of the ifeature is missing as there was a flange angled at 5 degrees. Also I am never sure whether to select "standard ifeature" or "sheetmetal punch"?

Re: iFeature extracting problem

Anonymous — Thu, 12 Apr 2018 19:35:52 GMT

Sorry I sent you the wrong one. Here it is

Re: iFeature extracting problem

jhackney1972 — Thu, 12 Apr 2018 19:36:26 GMT

The flange did not exist in your original post I responded too. Also to answer your question, you only pick a sheet metal punch option if you want to use it as a sheet metal punch in the sheet metal environment. It is the only one that must contain the centermark for placement.

Re: Using Ifeatures

jhackney1972 — Fri, 13 Apr 2018 01:08:29 GMT

What you sent out did not contain an iFeature so I took the liberty to suggest another method. It seems to me that your are looking for a sheet metal door that can be adjusted. The advantage of my method is that it gives a smooth radius to the door fold and the door top edge remains square to the face of the door. Take a look at the screencast. I have included the model.

If you truly want a sheet metal punch of this door, you will have to approach it in a different way. If this is the case, define exactly what you want such as the parameters you want to edit, what the punch is suppose to do, etc. and submit again.

Re: iFeature extracting problem

kelly.young — Mon, 16 Apr 2018 22:12:39 GMT

Hello @Anonymous how are you getting along with the iFeature? Did the file and screencast shared by @jhackney1972 get you any closer to what you're trying to accomplish?

If you can attach your .ide with the .ipt that would help.

Here are some of the better links if you haven't checked them out already:

AKN: iFeature fundamentals

AKN: iFeatures in designs

YouTube: Using iFeatures in Autodesk Inventor - Part 1

YouTube: Autodesk Inventor - Configured Design Tutorial | Creating iFeatures

YouTube: iFeature Design - Autodesk Inventor 2018

YouTube: Inventor 2012 sheet metal punch tutorial

YouTube: Inventor 2017 Sheet Metal Punch Updates (Skip to 1:30)

There are quite a few links, but each shows a couple of different tricks. It all come down to the setup and making sure everything is defined properly. Hope that helps!

Please select the Accept as Solution button if a post solves your issue or answers your question.

Re: iFeature extracting problem

Anonymous — Wed, 18 Apr 2018 15:48:30 GMT

Hi Kelly, I am still having problems with extracting the Ifeature. Inventor is now telling me that I have unsatisfied geometric inputs? I have attached my files below

Re: iFeature extracting problem

kelly.young — Thu, 19 Apr 2018 21:34:48 GMT

Hello @Anonymous thanks for attaching the parts.

The dialog box you're getting is wanting you to select the geometry first. Here is a screencast showing how to set it up a bit easier.

I haven't used the iFeature or Punch tool extensively in my work history, most everything I made was custom so didn't have a high use, usually just did for the dimple holes on the U-Haul auto trailers.

Maybe @S_May or @Thomas_Savage can share some of their sheet metal mastery on the subject!

Please select the Accept as Solution button if a post solves your issue or answers your question.

Re: iFeature extracting problem

S_May — Wed, 18 Apr 2018 18:04:57 GMT

https://knowledge.autodesk.com/de/community/screencast/1c748f61-b11d-4851-a1c7-5c2b04b1858b

https://knowledge.autodesk.com/de/community/screencast/ee70f15b-4d73-4115-a4f7-afee11ed1a6c

https://knowledge.autodesk.com/de/community/screencast/e18bc784-5c98-44a0-82b2-b363adffd509

https://forums.autodesk.com/t5/inventor-deutsch/inventor-ifeature-stanzwerkzeug-pragen-von-blechen/m-p/7406498#M5232

https://forums.autodesk.com/t5/inventor-deutsch/ifeature-im-maschinenbau-und-der-blechverarbeitung/m-p/7172946#M3758

@kelly.young..... Danke

Re: iFeature extracting problem

S_May — Wed, 18 Apr 2018 18:08:22 GMT

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/sfdcarticles/sfdcarticles/Including-a-work-axis-in-a-Sheet-Metal-Punch-iFeature.html

Re: iFeature extracting problem

johnsonshiue — Wed, 18 Apr 2018 19:33:27 GMT

Hi Kevin,

The Sketch3 has a projected edge from a workplane or an axis not participating in the extraction. Please delete it and project an edge from participating geometry (the one which will be part of the punchtool).

Many thanks!

Re: Using Ifeatures

Thomas_Savage — Wed, 18 Apr 2018 21:21:25 GMT

Hello @KevinPinks7697

@kelly.young Thanks.

I have looked at your .ipt.

Firstly you didn't fully constrain all your sketches. You need to always fully constrain your sketches.

I deleted a few projected edges and fully constrained your sketches. Which then allowed me to create a Sheet Metal Punch.

Secondly, as you can see i selected the Cut in the Extract iFeature. Which then selected the Extrusion. I selected theCut first as this contains the centre point. Which determines where the Punch is placed. If you select the Extrusion first then it will not work. As it can't find the Centre point.

The rest i have done in the Screencast. Creating the Sheet Metal Punch and placing it.

Is this what you wanted?

And have you anymore questions?

Thomas.

Re: Using Ifeatures

Anonymous — Fri, 20 Apr 2018 12:54:02 GMT

First of all, thanks for your help. How do I fully constrain the sketch if I cannot project any geometry. I am looking at the first cut sketch, which is not fully constrained, but I am not sure how to fully constrain it?

Re: Using Ifeatures

kelly.young — Fri, 20 Apr 2018 15:59:25 GMT

@Anonymous I can see how that is a bit misleading.

The rectangular cut isn't constrained but could be if you dimension the center mark or outside edges of the rectangle to the sheet metal plate. These projected lines from the plate won't be brought in because the iFeature is being located by the center mark and the dimensions to fully constrain the rectangle aren't referenced in the iFeature creation.

But if you reference the sheet metal plate in the creation of the lance it will cause problems which is why I showed how to Project Geometry from the Extrusion Cut being included in the iFeature authoring instead of the outside plate edge.

The whole statement about not including the Project Geometry is about the reference to anything not necessary for the iFeature, namely the plate itself.

Imagine the plate as an infinite plane that you are just defining your future iFeature on. As long as the cut/geometry fits on the plate and there is a center mark to locate it, the initial location doesn't require to be fully constrained (although it is still good modeling practice). The definition of everything after that should be Fully Constrained without referencing the plate edges for stability.

Hope that makes a bit more sense.

Re: Using Ifeatures

johnsonshiue — Fri, 20 Apr 2018 18:08:09 GMT

Hi Kevin,

You can project geometry. The issue here is that you cannot project non-participating geometry, since Inventor would not know how to establish the association. You can still project the edges created by the cut, which participates in the extraction. Does it make sense?

Many thanks!

Re: Using Ifeatures

Anonymous — Wed, 25 Apr 2018 12:59:15 GMT

Still having issues with Ifeature. Can someone please look at these files and let me know what is wrong?

Betreff: iFeature extracting problem

S_May — Wed, 25 Apr 2018 13:06:24 GMT

Betreff: iFeature extracting problem

Anonymous — Wed, 25 Apr 2018 13:13:35 GMT

What does that mean S May?