extrude feature help

[ctbram]

I am just learning inventor.  I have come from an artistic modeling background (Maya).  I am modeling a refirdgerator shelf baracket to be 3D printed and I am having trouble centering a work plane.  In the attached image I have a solid feature modeled and you can see the closed loop I want to extrude.

You can also see a centerline selected.  I want to extrude the feature an equal amount on either side of the center.

In retrospect I should have probably sketched the feature on a workplane that was already at the center line then extrude an equal distance symetrically.

But now I have what I have and I cannot figure out how to move the workplane and the sketch to the centerline or extrude the feature an equal distance across it.

Can any please help me salvage what I have or do I have to start all over?

[CCarreiras]

Hi!

You can "Redefine" the plane and place it in the right place.
If you already used that plane for other sketches, don't touch it.
Create a new plane center plane (you have a several ways to do that) and "redefine " the sketch instead.
To "Redefine" the plane or sketch definitions, just RMButton over them in the browser tree and select Redefine. Just select the new specifications.

[ctbram]

oops I should have probably mentioned I am using inventor 2016.  RMB over either the sketches or the workplane in the browser tree I do not see "redefine"

[ctbram]

Okay,

Thanks for the help so far.  I have managed to get to the point shown in the attached screen shot. 

Now the problem is my browser tree has Sketch 10 in it twice and they seem to be linked.  Can I unlink them and delete the sketch that is outside of Extrusion 3?  It's confusing to me having that sketch show up twice.

What I did was to create a properly centered work plane.  Then I selected the four skectch lines forming the solid feature outline and projected them ointo the new workplane.  Then I selected the old workplane and all the sketches I drew on it and deleted them.  I had to uncheck delete dependent features (or something like that).  I ended up with what you see below in the browser tree. I'd like to clean up the duplicate Sketch 10.

[ctbram]

Here is the next issue.

I am hollowing out a shell in the upper section of the bracket.  But as you can see it goes down into the clip at the bottom.  How can I instruct inventor not to shell that section of the part?

[CCarreiras]

Hi!

You can find Redefine Here:

[CCarreiras · Accepted solution]

Hi!

The Sketch is repeated because you shared this sketch with several operations.
To do that, probably you activated "Share Sketch". When you able "share sketch", (or put the sketch visibility "on" after using it in one operation) the sketch will come outside the operation and is ready to be consumed by other operation, like a cut or something else.
If sketch 10 is only used in the extrusion 3, RMB in the sketch and mark "UNSHARE". The outside sketch will disappear.
Note: You can not unlink the sketch, because both are the same. This is a normal behavior, get used to that.

[CCarreiras · Accepted solution]

To do this shell, i think the easy way is use multisolid option.

Edit your extrusion 3 and point it to "new solid"

You will have a multisolid. Perform the shell in the new solid. The feature only will occur in the solids you choose.

After, unite both solids with a boolean operation... use combine.

Check the video, will explain all your last questions.

[CCarreiras]

Back to the begining....

i saw you dont have the sketchs fully constrained... this is very important.

Also, why you use a new plane? (Work plane 2) why dont you use again the center planes? the same you use for the first feature?

Somthing like:

First feature: skecth in the xy plane: extrude both sides.

next feature (extrude 3): select the same plane and again extrude for both sides.

This way, you have the part centered and without extra work planes...

[ctbram]

Thank C.

Yeah I realize that I have extra planes.  I am very new to inventor and I started the model the wrong way.  I was working from an image and it put the initial image into a quadrant and I did not know how to center it on the grid.  Then I built the clickp profile and extruded it styraight up.  Then realized I needed to build the second feature but the initial work plane was in the wrong place.  Rather then start over I just built it from a workplane (in the worng place). and  then I had to create another workplane in the right place and project the sketch for the second feature.  Then delete the other workplane and sketch. So the enitre project has been a cascade of errors and cludges to fix them.

[CCarreiras]

You dont have too much work done yet, you can start again in the proper way fast and easy.

If you will, you can send me the file and i help you, or show you how to do it...

[ctbram]

by the way if the extrusion3 is already part of solid1 can I extract it into a new solid.  Make the shell and then recombine it or do I have to delete the extrusion and do it again the way you show in your video?

and yes I could just start all over but this part is close to donw.  I just neeed to shell the upper feature and extrude two pins.

I was hoping to get something to 3d print and then redo the model on the weekend and do it the right way.  I am learning the workflow and although there are lots of videos on youtube I just have not had the time to spend running some of them to learn the proper workflow for things.

[CCarreiras]

Yes... edit extrusion and change it to "new solid"

[ctbram]

Super!  Thanks for all the help.

It's almost done.  I just have to combine it, extrude some posts, add some fillets, and fix the constraint issue and I will have something I can 3D print.

I do plan to redo this as an exercise and do it the right way.

Thank you,

Rick M

[JDMather]

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@ctbram wrote:

I do plan to redo this as an exercise and do it the right way.

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That should take about 3 minutes.

Attach the file here and someone will do it for you.

[ctbram]

Thanks but part of the reason I am doingthis is to learn.  Aside from he clip part that requires splines the rest should be very easy I agree.  I come from an entertainment 3D modeling background mostly Maya.  In Maya I can make a part that looks right in about 10 minutes.  

But this is a real part that I hope to 3D print to replace a broken piece in my refridgerator and therefore needs to be more accurate.  I have been wanting to learn either inventor or solidworks so I thought this would be a good way to do it.

It's simple enough that if I have to start over a couple times it would not be a major issue.

Thanks again for the advice and all your help.

-Rick

[JDMather]

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@ctbram wrote:

Thanks but part of the reason I am doingthis is to learn.  

-Rick

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One of the powers of Inventor - it is a history based modeler.

Reading the sketch/feature history tree of an expert created part would be better than reading a book.

And if others could read the history of how you were attempting to create the part - they can show you an poor modeling techniques you might be picking up into poor modeling habits.

My suggestion to you to post your file was not a result of careless thought, it comes from years of teaching others how to use Inventor (and other CAD programs).

[ctbram]

ah IC.  I thought you were suggesting others do the work for me.  But I see your point and will certainly post the ipt file.  I have attached it below along with some images of the part I am trying to build for 3D printing.

Thank you,

Rick M

Here is a link to some reference images.  The post you see is at a 90 deg angle ie perpendicular to the open side and there are two of them.  They both snapped off and the one you see in the reference images is just tacked in place to show the configuration.

http://imgur.com/a/FQTk8

and attached is a copy of the ipt file.  I definately did a bad job on work flow and have not redone anything so you can see the process of fixing and cludging as I stumbled along.  There are no contraints yet as I had no calipers as I build this and planned to add contraints when I could get it in to work where I have some calipers to properly measure things.

The illustrator line view is to scale though so it gets some of the model close to the right dimensions.

I am kind of stuck at this point trying to figure out how to model the two posts that come out in the corners.  I was thinking a work plane parallel to the open suface and then extruded down and joined to the inside angled face and then somehow cleave off a angled bit to create the part that comes to a point at the top.

Thanks all for your assistence,

Rick M

[CCarreiras]

Hi!

You have special tools to do that.

Search in Plastic Parts Tab.

Make a New plane (Offset from xz)

Create a sketch, only with 2 points.

Use the tool Boss and selerct thread mode.... Then... just fill the fields properlly.

[ctbram]

I'll look into that but I am not sure it will be appl;icable.  

The two pins fit into the aluminum rail of the rack.  The part I am modeling is a cap at each end.  The V shape of the pin fits into folded groves in the top and bottom of the aluminum rail.  The boss tool looks like it creates the ribs symetrically.  I need just two ribs but they need to be at something around 45deg.

 Here in my album you can see how the cap I am modeling fits into the rack railing.

http://imgur.com/a/FQTk8