Simple hole with a pocket for a nut for 3D printing.

[mailswamp]

Hello.
I use Inventor 2022 and I have been using it for years mostly to design one-off parts like this:

 and to 3D print them. I had no need to do more complicated things untril very recently.

I am trying to design an iFeature that would allow me to create a hole with a pocket for a regular hex nut to slide into so I could attach a lid to a 3D printed part using many little screws.

I would like to enter the location of the hole by providing the references of Point1 and a Plane1 and perhaps another Point2, to define which way the pocket hole would face. Unfortunately I could not get Inventor to use a point as a reference for how deeply into the part from Plane1 (the mating surface), the nut pocket would be placed, as well as the angle that it would point at. What should I use to define those parameters?

I am fine with using numerical values, yet what do I reference to define the angle of the pocket?
I would like to design this iFeature to also work with organic surfaces.

I could not enter this iFeature so it would work correctly.

How do I ensure that the pocket is aligned with the center of the hole, swivels around this center axis, while allowing me to choose geometry to reference the angle of the pocket, into which the nut will slide into?

What would be the best way to define the distance of the pocket hole from the Plane1 (that would also contain Point1)

For some reason, when I tried to specify the angle of the pocket to one of the provided axes that stem from the origin, my iFeature would no longer want to reference the Point1 and would randomly appear anywhere on Plane1.

What should I do?

Do later versions of Inventor contain fewer bugs and offer a more straight-forward process for the creation of an iPart?
For example, to play with settings I have to select things in this tiny window with a scroll bar and I cannot enlarge it.

 Screw Pocket M2 test is the file that I am using to generate the iFeature.

The reason I did not make a through hole was so I could use the depth of the hole to determine how deeply I would like to set in my pocket. This was a work around since I could not specidy how down far from Plane1 I would like to have my nut pocket.

I watched many tutorials on the subject before asking this question.

Also I am having a difficulty attaching I feature .ide files.

How can I attach them?

Thank you.

[johnsonshiue]

Hi! You may zip up the files and attach the zip file. Regarding positioning an iFeature, there isn't a workflow snapping the iFeature to a sketch point. Depending on how the iFeature was built, you might need three planar references to lock the location on placement. Please share the files in zip here. I would like to take a look and understand the behavior better.

Many thanks!

[mailswamp]

johnsonshiue, thank you for reminding me that the software is a little more limited than my wishful thinking about what it could do. I wish I could work as a beta-tester for Inventor to optimize its interface.
Many of my designs are workarounds around known hangups. Like I know that it would be difficult to select or to configure something three steps ahead so I go a different route. I still like Inventor more than other CAD software of the same class.

I attached the files in an archive.

Most tutorials don't seem to go into such specifics like how to make  a practical lock and I have several such locks to design if I want to make parts that have more than one piece. Even my $400 course did not spend too much time on such specifics.

In this case, both of the features are subtractive. They remove material to make holes.
Would it be possibe to turn the features that are involved in this iFeature into a solid that I can subtract from the part that I am designing by giving it some references?

Sometimes I wish that the positioning when I work within the part environment worked a little bit more like the positioning of parts in the assembly, which is what my next question is going to be about.

I experience some fuzzy logic with the variations of the iFeature that I created because when I add a request for the reference for the pocket hole location, the entire iFeature begins to ignore the point as a centerpoint reference and wanders away as I try to give it references.

I need to place those bolt connections on points. This iFeature needs to work like the hole command in order to be handy. I am also not sure what the alternative would be if I want to recreate this thing in many parts without having to redraw it every time.

[JDMather]

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@mailswamp wrote:

 I wish I could work as a beta-tester for Inventor to optimize its interface.

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>>Beta Testing<<

[JDMather]

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@mailswamp wrote:

1. Would it be possible to turn the features that are involved in this iFeature into a solid that I can subtract from the part that I am designing by giving it some references?

2. Sometimes I wish that the positioning when I work within the part environment worked a little bit more like the positioning of parts in the assembly, which is what my next question is going to be about.


3. I need to place those bolt connections on points. This iFeature needs to work like the hole command in order to be handy. 

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@mailswamp 

I just want to give you some encouragement.

Now that I am retired I have other more important (to me) things to get done - so I don't have time to recover old work.  But I encourage you to keep working on it - this is easier than you might think.  You have at least two options.

1. Yes.

2. The Direct Edit > Move can be used similarly to assembly constraints - but takes some practice to get the hang of it.  In the past I have posted a video on this technique.

3. Some 15 years ago I presented a paper on how to do this using a trick with the Sheet Metal Punch Tool. 

You have to temporarily fool Inventor by toggle Sheet Metal/Standard, but that is easy enough to do.  In my demo I specifically targeted use with organic shapes.

Edit: I took a look at your file.  You have too many dependent references.  You want only two dependent references - a sketch point and a face.

[Frederick_Law]

A quick try of iFeature

The hole is easy.  Problem is slot.  May need to think outside the box.

Maybe, cut round, cut square below round, cut to wall.

[johnsonshiue]

Hi! I did not modify any feature. But, when I extracted the iFeature, I did add the three reference lines to the geometric conditions. I am able to insert the attached iFeature by picking the two sides of the square, picking one side again, and picking the face.

Please take a look at the attached ide file.

Many thanks!

[mailswamp]

JDMather, I also noticed that the punch tool works a lot better than the iFeature to do roughly the same thing.

Thank you for confirming this observation.

About 1): would it be possible to produce an "iFeature" using a series of overlaid, aligned additive and subtractive operations? For example: a simple lock that creates interlocking geometry in two plastic parts.

Would I have to reference or align all of them by hand?

Can I insert them as a parametrized solid or a series of parametrized solids that are all linked to the same parameters and can be changed all at once via an excel table, for example?

About 2): I use position a lot when I work with multi-body parts. Unfortunately, I find it difficult to rotate the part placed into another to the right position since there is no rotate included with this 1980s looking Move Bodies function. I know that there is a workaround with patterning solids, yet this workaround adds more confusing operations into the model tree and increases the complexity of the part.

I may have to upgrade my part to an assembly because the choice of tools for positioning in the multi-body part environment make everything very confusing.

Since there is no convenient way to generate real geometrical threads for 3D printing, I would like to generate virtual tap bodies that I can drop on a center axis and than use a subtractive technique to produce threads.

I occasionally want regular metric screws to thread into plastic, yet I also have my own screw designs that are optimized for 3D printed screw mechanisms where both parts are 3D printed.

What would be the best way to do this?

3) Is this workaround with Sheet Metal still relevant in AI2022?

My iFeature has to be converted to a punch when it is created do I need to turn that cube of material that I used to generate it into a 'sheet of metal' or am I temporarily turning a part that I am punching with this punch into a piece of 'sheet metal', or both?

Thank you! Maybe this is as good as it can get.

I am surprised that there are no hundreds of tutorials in existence on how to make such locks.

johnsonshiue
Ideally, I have to reference three things - axis, depth of the pocket and the direction angle for the pocket to exit the part (generally - towards the nearest outside surface, yet sometimes it helps to be able to adjust the angle)

It looks aligned. Yet when I insert it, it appears on the outside of the part which made me flip it, causing it to fail the first time.

It seems that the feature appears at a random location and I cannot snap it/ reference it to a point or on an axis.

 

By playing with your model, I finally figured it out, recalling a tutorial that mentioned that features only work when referenced to axes and realizing that I cannot use any axes of my own so I have to rely on the three ‘officially’ provided axes: the X,Y and Z.

For future reference: I generated my feature from a block that was sketched around the official vertical Y axis:

I wish that I could specify that Point1 input is to be the same as Point2 instead of selecting them independently every time.

Also I specify depth of the nut pocket with a dedicated plane but this may not be the worst way to do it, considering all the limitations of the I feature reference data input.

things don't look to scale because I did not specify realistic dimensions of the bolt and a standard nut yet.

I could, as pineapple.law1972 suggested, use a workaround and cut a round hole to a desired pocket depth, reference pocket depth to the bottom of the hole, than cut another hole over it, past the pocket, to a desired depth.

Fortunately, the pocket extends into space as it slowly angles out and I can make it arbitrarily long.

I give the pocket a line reference for direction (does not matter if the line is on the same plane - even more convenient)

Does the creation of iFeature work as clumsily in 2023 version as it does in 2022?

I was not able to open files in the Pocket-iF folder because of this:

 

Is there a quick way to reduce compatibility mode or to save a file for an older version of Inventor?

@johnsonshiue @Frederick_Law @JDMather Thank you for your time and for guiding me towards finding the answer. I am yet to try this with complicated organically-shaped geometry.

All my files are included in the archive Pocket Hole 02.rar

[mailswamp]

Update:
Now I am struggling with placing the cutout iFeature into the model that I am designing.
There is not a convenient way to see the geometry before I place it.

In some cases, when editing the iFeature references, I could see that a geometry like this is generated:

The original sketch is fully referenced.
This seems like a bug in the software.
If I do not refer the sketch angle to an axis, as here with the 30 degrees, I do not get an option to choose a line reference for direction of the pocket when I generate an I feature. Is this a bug?

How do I allow myself to choose a direction for the cutout to face without having those issues that my fully referenced sketch gets distorted as I use this iFeature?

VS:

And than it turns into this necktie shape because it tries to reference a X or Z that is not there.
My sketch is not referencing axes, other than Y that pierces through the center of the hexagon and is the centerline for the round hole.

I was able to experiment on a simpler part, yet I got similar results - either I have to specify an angle and deal with issues or not have control over the angle that it is pointing in.

I turned off the visibility for the bodies that were getting in the way and I got this:

Another update:

pocket holes are exposed because I reference the plane for the pocket hole depth as the outside plane of the lid.
I am being lazy. If I create a dedicated plane, I can move the pocket up.

It seems that it was easier to define an extrude cut between two dimensions, referenced from a plane in the older versions of Inventor. Was this improved in 2023?

Sorry, I cannot show all the position geometry in this screenshot because of this (in my opinion totally unnecessary) scroll bar.  Enter_Angle_TO_Line can be set to 0.
I was able to use it on my humidifier and enter the value of 180 degrees into the prompt for Enter_Angle_TO_Line  to flip the cutout pocket the right way.

Thank you for your time. Let me round up all the files that can be useful for educational purposes after the break.

[cadman777]

How about cutting round down to the bottom of the nut slot, and then add the slot to the center of the bottom of the hole?

I've made nut pockets for 3d printed part in Inventor, but manually. By way of design, one thing I did that the OP doesn't seem to be doing is make the hole deeper than the nut pocket so there can be a little overshoot of the screw. That's typically what you want when you use fasteners to be sure you get all the 'good' threads captured in the fastener connection.

[mailswamp]

My hole goes straight through.
I can make it overshoot to a specific depth.
However
what if I drop something in the hole and clog it. I avoid blind holes in my designs if possible.

my current pocket hole works well

if I add more features to it, I will probably have an even clumsier iFeature with even more parameters
the combine feature sometimes does not work very well.

I end up having to enter the same point twice.
I wish I could edit the iFeature capture input instead of doing it again if I want to change something.

This is the part that I used to generate my new pocket hole.
I extrude a cylinder instead of a cube.

It seems that creating it on the round surface allows me to input a curved and a straight face, while if I create it on a straight face, I get an error when I try to use it on a curved face.

I may also design some nut shoots that are angled and have a curve.
I may also create a channel to extract the nut with a wire to save money on hardware.
Yet it seems that iFeatures quickly become unstable and difficult to work with.

Is there any way I can subtract a solid to produce a set of holes like this?