iFeature extracting problem
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.
John Hackney, Retired
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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.
John Hackney, Retired
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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.
John Hackney, Retired
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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:
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.
Kelly Young
* Ideas * Help * AKN * Updates * Pack & Go * Reset Utility * Repair Install * Customization * iLogic Examples * Autodesk University *
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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.
Kelly Young
* Ideas * Help * AKN * Updates * Pack & Go * Reset Utility * Repair Install * Customization * iLogic Examples * Autodesk University *
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!
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.
Thomas Savage
Design Engineer
@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.
Kelly Young
* Ideas * Help * AKN * Updates * Pack & Go * Reset Utility * Repair Install * Customization * iLogic Examples * Autodesk University *
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!
