Extrusions in assemblies, and parameterization based on existing parts

[newcomer]

I've included a simple set of drawings that illustrate my problem.

Sensor Unit.ipt is an ultransonic sensor transducer mounted on its control board.

Sensor Case.ipt is the case into which this transducer will be mounted.

Sensor Assembly.iam is the assembly in which I put these two pieces together.

Now here's the set of problems I need to solve:

(a) If you look at the Left side view of Sensor Assembly.iam, you will see that the sensor protrudes beyond the work plane.  The work plane is placed where the cover front will be.  What I want to do is constrain the front of the sensor transducer to be mated to the work plane.  However, that does not seem to be one of the options for which mating works.

(b) Given that I have mated the sensor to the work plane, I now need to create two bosses (actually, all I need is a circle extruded with a 5-degree expansion) that run from the back of the circuit board to the wall of the case behind/below it.  These will have a hole in them that will be tapped by a 4-40 tap.  The problem is that when I place a work plane on the bottom of the circuit board, and try to extrude "To" the case, it will only let me do a "cut" extrusion, which is useless.

What I am trying to do is remove a circular dependency, wherein I would put the bosses on the case (Sensor case.ipt), and have to keep adjusting them based on where I have to put the parts to meet clearance requirements.

If I go to the assembly and move the Sensor Unit, I want the bosses to move with it; I don't want to have to go back to the case where the bosses are drawn and move them to match.

Another idea that might work is if I can take a unit and make it a "construction object", that is, it looks like construction lines.  If I want to print the part so I have a little plastic simulation of the object, then I need it as a drawing.

What I want to do is "hide" the Sensor Unit.ipt part of the drawing, so when I 3D-print it, I have only the case and bosses printed.  Right now, I can't seem to get it to print only the "Visible" parts, in spite of the fact that the print dialog offers me "All Visible" or "Selected".  I would have thought that "All Visible" meant "Visible", and a part whose visibility I had turned off, which is clearly "not visible", would not be included in the print.

Next, I need to create a cover for this case, which is a simple rectangle with filleted edges on its top, and a hole properly placed for the acoustic transducer.  If I move the Sensor Unit.ipt part around in the assembly, I want the hole in the cover to follow its movement, so when I print the case and cover, everything will fit.

[Note that I did not include the bosses for holding the cover on in this set of files; I consider that to be an unnecessary complication for this submittal]

What I have done is make each key parameter (those derived from the basic specs of the problem) to be a "User" parameter, and exported; internal parameters may be named, but they are coupled to the user parameters.  In a programming language, the User parameters would constitute the "visible" interface to a module, and the Model parameters would constitute the "private" or "hidden" components of the module.  So that is the mindset I'm coming from.  I use the Link option in the parameters as the equivalent of the "#include" feature of C/C++ (if this helps you understand what I'm trying to accomplish).

How is something like this normally handled? (Again, as a beginner, my problem is trying to figure out how to think about these problems; my temptation, after 50 years in the software development business, is to try to modularize the parts and assemblies so they can be recombined in various ways--creating a library of parts).

And that raises another issue.  Suppose I have a part which has a dimension that cannot be determined until it is included in an assembly.  For example, an internal support that should be (case_depth - case_thickness) in height.  But I want to use it, as a library component, in several different cases, each of which has a different depth.  In effect, how do I create a part with an "unbound" parameter which I do not bind until I place it?  I don't mind if I have to set it to some predefined value, such as 5mm, which is too short for any case, but will obviously need to be set.

Feel free to point me to Invertor documentation--I find it hard to search for an answer to a question since I do not yet have the "vocabulary" of Inventor in my head at this point.

thanks much

joe

I am now using Inventor Professional 2014; Techshop upgraded their machines this week.

[PaulMunford]

There's lots of questions in there - I can't answer them all right now (from my phone), I'm sure others will help out!

For adaptivity try this posts from Curtis Waguespack:
http://inventortrenches.blogspot.co.uk/2011/05/isolate-before-assembly-features.html?m=1

Assembly level features only effect the assembly - so they won't appear in the part file.

You could link the features using derived tools:
http://au.autodesk.com/au-online/classes-on-demand/class-catalog/2013/product-design-suite/ma2604

Any parametric part can be used as a library part and resized once placed inside assembly - but you will need to create a copy of it first.

One easy way to do this is to save it as a template part in your template file location.

IT sounds like you might enjoy using iLogic (inventors VB.net based scripting language.) Here's a good place to start:
http://inventortrenches.blogspot.co.uk/2013/10/ilogic-how-to-learn-inventors.html?m=1

you can also use iLogic to 'push' values down from the assembly, so that you can create relationships between parts without having to link or derive:
https://www.google.co.uk/url?sa=t&source=web&rct=j&ei=CN_bUuObErT70gW7toH4DA&url=http://m.youtube.co...

Keep trying, let us know how you get on and come back to us with any specific questions 😄

[JDMather]

I get an error trying to extract the *.zip.
Anyone else seeing this problem?

[JDMather]

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@Anonymous wrote:

(b) ...  The problem is that when I place a work plane on the bottom of the circuit board, and try to extrude "To" the case, it will only let me do a "cut" extrusion, which is useless.

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For some reason I cannot extract your assembly to answer questions directly one-by-one, but from this description

you are trying to add an assembly level feature.  Just like in the real world, when you have assembled parts you can only remove material, example - match machining, drilling hole through both parts at same time.

You need to edit the part in the context of the assembly and then Project Geometry or Copy Object to use geometry from one part to control geometry in another part.  But all of this is advanced techniques that in my opinion most users should have expert level of proficiency before attempting.

There is a much easier technique.

Learn multi-body solids master modeling techniques within a single part file and then push out the assembly (Manage>Make Components) when done.  This is a much more robust technique. And did I mention that it is easier?

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf
http://inventortrenches.blogspot.com/p/inventor-tutorials.html
http://wikihelp.autodesk.com/enu?adskContextId=HELP_TUTORIALS&language=ENU&release=2014&product=Inventor

[rdyson]

JD, I was able to open it with winrar. Attached is a new zip, hopefully it'll work for you.

newcomer,

JD did, or will provide liks to his and other tutorials. I strongly suggest you spend a day going through them. It save you weeks of fustration.

In the meantime:

a) I don't know what the "front" of the sensor means but I suspect you wat to use a flush mate between the black surface ane the work plane.

b) You need to edit in palce the sensor case. Either double click it in canvas or RMB in the browser. If you create your sketch plane selecting the bottom surface of the sensor board, it will become adaptave and will adjust with changes to the boards height. Be advised that adaptivity can lead to far more problem than it cures, especially for the new user.

[JDMather]

On your Sensor Case part I recommend you add the external fillets and THEN Shell the part.

As it is now - your wall thickness is not uniform (not good for a plastic part) and I would add a bit of draft angle to Extrusion 1.

[JDMather]

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@Anonymous wrote:

(b) Given that I have mated the sensor to the work plane, I now need to create two bosses (actually, all I need is a circle extruded with a 5-degree expansion) that run from the back of the circuit board to the wall of the case behind/below it.  These will have a hole in them that will be tapped by a 4-40 tap.  The problem is that when I place a work plane on the bottom of the circuit board, and try to extrude "To" the case, it will only let me do a "cut" extrusion, which is useless.

What I want to do is "hide" the Sensor Unit.ipt part of the drawing, so when I 3D-print it,

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The The

The case needs to be edited to include the bosses (at the part level, or at the part level in context of the assembly).  I would use the Boss tool on the Plastic feature tab.

Hiding a part does just that - it still there.  I think what you want to do is right mouse button Suppress the part

or

open the part file separately to save to *.stl for printing.

[newcomer]

The most promising link unfortunately seems to insist on the Adobe Flash Player. Why a proprietary choice was made instead of one of the numerous open standards for video was chosen escapes me. It is worth noting that not all devices are even capable of running Flash (e.g., iPads), and my desktop, which has Flash installed, gives the same error. This strikes me as very odd.