Inventor General Discussion

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killbox
Posts: 20
Registered: ‎01-26-2013
Message 1 of 10 (2,686 Views)
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Moving solids in multi-body parts

2686 Views, 9 Replies
01-26-2013 08:52 PM

I am new to Inventor Pro 2013.  I have 17 years of Unigraphics / NX and 2 months of AutoCAD 2013 3D experience .  I am designing a welded table that has lots of tubes to be aligned to each other.  It appears that snaps do not work on solids and there is no way to do a point to point solid move in Inventor.  Is there any way to select a solid, snap to a base point, then move or copy to a snap destination point of another solid?  Does this need to be done in an assembly drawing?  If so, do I have to create a file for each tube and then bring each of them into an assembly?  I would like to draw the table as one part.  Designing all the parts together.  The lack of snaps is strange to me.  I can only snap to end points in sketches.  No midpoints??  I must be missing something very basic and easy.  I have not tried an assembly drawing yet.

 

 

I have been working through hours and hours of training videos.  Everything but move, copy and paste has been pretty easy.  I think I need to find an AutoCAD to Inventor transition video.  There are no training courses in my area.  So I'm stuck with online training.  This problem is never addressed and I can't ask the question on a video.

Hi killbox,

 

Okay, take a deep breath ... hold it ... let it out slowly ... and then repeat these words 10 times:

 

  1. "Inventor is not AutoCAD"
  2. "Inventor is not AutoCAD"
  3. "Inventor is not AutoCAD"
  4. "Inventor is not AutoCAD"
  5. "Inventor is not AutoCAD"
  6. "Inventor is not AutoCAD"
  7. "Inventor is not AutoCAD"
  8. "Inventor is not AutoCAD"
  9. "Inventor is not AutoCAD"
  10. "Inventor is not AutoCAD"

:smileywink:

 

I'm taking a break from my own project where I've been having trouble getting my mind around a new tool that is similar but different than what I'm used to :smileyfrustrated:, so I know where you're coming from. I also used AutoCAD extensively before moving to Solidworks and then Inventor, and found that it was at first hard not to try and do things like I would have in AutoCAD.

 

So with that in mind, try a new approach for your sketching, and I think you'll find that the need to move things around is rarely required. Create a very simple sketch and extrude it to define the bounds of your router table. Then sketch on the various faces of the box to create bracing and cross members.

 

So rather than trying to create "stick" sketches like this:

 

Instead create a 3D solid like this:

 

 

And then sketch on the faces of the solid such as this :

 

 

This way you're creating the sketch right where you want the sketch in the first place, so there is no need to Move, Rotate3D, Snap, etc.

 

And take JDMather's advice to reuse your existing sketches as much as possible by projecting geometry.

 

Also keep in mind that to start off it typically helps to think about creating your models the same way you would in the real world. That means if you have a screw in your assembly, then you will have an *.ipt file for that screw, if you have a steel gantry plate for your router then you'll have an *.ipt file for that, and so on. Each part in real life has it's own *.ipt file, that you'll put together in your assembly file. If you reuse the same part in the real life assembly, then you just do the same thing in your Inventor assembly (ex: two instances of the same gantry plate).

 

Of course you can cheat a little bit, for instance your stepper motors are obviously assemblies in and of themselves, but you typically wouldn't model it as seperate parts, unless you're intending to manufacture a stepper motor.

 

Same thing with the guitar. The body is a one part, the neck is another, same for the pickups, same for the bridge, all are modeled as part files and then put together in the assembly.

 

Once you master the one part = one part file approach, there are other modeling approaches that work more like AutoCAD where you create parts from seperate solid bodies, but start off learning the rules of working in Inventor and then you can learn to bend them to your will using more advacned strategies.

 

One last tip, keep your sketches simple and you'll find Inventor is much more friendly:

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

*Expert Elite*
Curtis_Waguespack
Posts: 2,963
Registered: ‎03-08-2006
Message 2 of 10 (2,663 Views)

Re: Moving solids in multi-body parts

01-27-2013 07:21 AM in reply to: killbox

Hi killbox,

 

It sounds like that working in Assembly is probably the best solution, but you can use the Move Bodies tool to do what you ask about:

http://wikihelp.autodesk.com/Inventor/enu/2012/Help/0073-Autodesk73/0308-Parts308/0393-Part_fac393/0...

http://inventortrenches.blogspot.com/2011/06/change-origin-of-imported-model.html

 

It might be a good idea to stop and run through the built in Tutorials, so that you have a better understanding of how Inventor works, otherwise you might keep banging your head against the "Inventor is not AutoCAD" wall.

http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126

 

Of particular interest to you for your weld table will be the Frame Generator tool (found in the assembly environment):

http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/0127-Inventor127/0721-Frame_Ge7...

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com



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Contributor
killbox
Posts: 20
Registered: ‎01-26-2013
Message 3 of 10 (2,654 Views)

Re: Moving solids in multi-body parts

01-27-2013 08:56 AM in reply to: Curtis_Waguespack

Curtis,

 

Thanks for all the good info!  The attached CNC router picture is what I'm currently trying to model.  The guitar will be the next inventor project.  Both were designed in AutoCAD 3013 / Showcase with just weeks of playing around with it.  Tools like 3d move, rotate, copy and paste with snaps made quick work of the frame.  I've tried the move bodies command in Inventor.  However, it does not give me snap points.  Dragging a part around with no snap does me no good.  I simply want to draw a tube and drag it in place using a snap.  I've used many solid programs and they all had a way to do that.  Coming from a Unigraphics solid modeling background I figured Inventor was what I wanted, not AutoCAD.  I thought it would be much quicker and easier than what I had used in the past.  Not looking good so far.:smileyfrustrated:

 

I'll look at the tutorials you posted.  I'll get the hang of it . . .  it's just taking a little longer than I expected.  Given the picture, how should I start the router table.  I figured the frame would be first, and I thought it should be one part file.

 

*Expert Elite*
JDMather
Posts: 27,601
Registered: ‎04-20-2006
Message 4 of 10 (2,635 Views)

Re: Moving solids in multi-body parts

01-27-2013 10:21 AM in reply to: killbox

In addition to the built in Help>Learning Tools>Tutorials and Skillbuilders

you might read this

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf

and this older more complete document

http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

and these

http://inventortrenches.blogspot.com/p/inventor-tutorials.html

 

The big difference in Inventor history-based modeling is that you can build intellegence into your models.

But this functionality requires significant up-front planning or experience.

Once you get the experience you will find that it all comes pretty logical and easy.

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2014 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015-SP1 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
Contributor
killbox
Posts: 20
Registered: ‎01-26-2013
Message 5 of 10 (2,619 Views)

Re: Moving solids in multi-body parts

01-27-2013 01:27 PM in reply to: JDMather

After going through the tutorial, the frame creator looks like it will do exactly what I want.  So I started the attached sketch.  Again, I run into the same problem over and over.  I sketched the top (sketch #1), then the side (sketch #2).  The other side is exactly the same so I copy sketch #2 into Sketch #3.  Now I just need to move Sketch #3 into position.  No snap?  Stuck again!  I'm doing something wrong.  Why did I have a snap to connect Sketch #1 to #2?

 

I've been through hours of tutorials and they never address this issue.  I get everything else.  How do you move stuff in this program? 

*Expert Elite*
JDMather
Posts: 27,601
Registered: ‎04-20-2006
Message 6 of 10 (2,602 Views)

Re: Moving solids in multi-body parts

01-27-2013 03:07 PM in reply to: killbox

Sketch3 is on the wrong plane and is unneeded duplication of work.

Create a workplane using endpoint and line from Sketch1.

Start Sketch3 on this workplane and then Project Geometry Sketch2 onto Sketch3.

 

Also you have too many dimensions. (I turned off the dimension visibility from Sketch1 to avoid confusion.)

Do not duplicate dimensions.

Use Equal (=) and Symmetry constraints.

Model with obvious symmetry about the Origin Center Point.

 

Frame Skeleton.JPG

 

Assuming you have used AutoCAD this is similar to changing UCS in AutoCAD to draw (sketch) on another plane.

The key is you must do this before sketching, you can't simply move (actually you can, but that takes more work than needed).

 

Whenever you need to connect one point (or line) from one sketch to a point on another sketch (similar to Osnap) use the Project Geometry tool to generate a parametric connection point.

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2014 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015-SP1 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
*Expert Elite*
Curtis_Waguespack
Posts: 2,963
Registered: ‎03-08-2006
Message 7 of 10 (2,591 Views)

Re: Moving solids in multi-body parts

01-27-2013 03:22 PM in reply to: killbox

Hi killbox,

 

Okay, take a deep breath ... hold it ... let it out slowly ... and then repeat these words 10 times:

 

  1. "Inventor is not AutoCAD"
  2. "Inventor is not AutoCAD"
  3. "Inventor is not AutoCAD"
  4. "Inventor is not AutoCAD"
  5. "Inventor is not AutoCAD"
  6. "Inventor is not AutoCAD"
  7. "Inventor is not AutoCAD"
  8. "Inventor is not AutoCAD"
  9. "Inventor is not AutoCAD"
  10. "Inventor is not AutoCAD"

:smileywink:

 

I'm taking a break from my own project where I've been having trouble getting my mind around a new tool that is similar but different than what I'm used to :smileyfrustrated:, so I know where you're coming from. I also used AutoCAD extensively before moving to Solidworks and then Inventor, and found that it was at first hard not to try and do things like I would have in AutoCAD.

 

So with that in mind, try a new approach for your sketching, and I think you'll find that the need to move things around is rarely required. Create a very simple sketch and extrude it to define the bounds of your router table. Then sketch on the various faces of the box to create bracing and cross members.

 

So rather than trying to create "stick" sketches like this:

 

Instead create a 3D solid like this:

 

 

And then sketch on the faces of the solid such as this :

 

 

This way you're creating the sketch right where you want the sketch in the first place, so there is no need to Move, Rotate3D, Snap, etc.

 

And take JDMather's advice to reuse your existing sketches as much as possible by projecting geometry.

 

Also keep in mind that to start off it typically helps to think about creating your models the same way you would in the real world. That means if you have a screw in your assembly, then you will have an *.ipt file for that screw, if you have a steel gantry plate for your router then you'll have an *.ipt file for that, and so on. Each part in real life has it's own *.ipt file, that you'll put together in your assembly file. If you reuse the same part in the real life assembly, then you just do the same thing in your Inventor assembly (ex: two instances of the same gantry plate).

 

Of course you can cheat a little bit, for instance your stepper motors are obviously assemblies in and of themselves, but you typically wouldn't model it as seperate parts, unless you're intending to manufacture a stepper motor.

 

Same thing with the guitar. The body is a one part, the neck is another, same for the pickups, same for the bridge, all are modeled as part files and then put together in the assembly.

 

Once you master the one part = one part file approach, there are other modeling approaches that work more like AutoCAD where you create parts from seperate solid bodies, but start off learning the rules of working in Inventor and then you can learn to bend them to your will using more advacned strategies.

 

One last tip, keep your sketches simple and you'll find Inventor is much more friendly:

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com



  solution.png  Did you find this reply helpful ? If so please use the Accept as Solution or  Kudos button below.





Contributor
killbox
Posts: 20
Registered: ‎01-26-2013
Message 8 of 10 (2,505 Views)

Re: Moving solids in multi-body parts

01-28-2013 08:34 PM in reply to: Curtis_Waguespack

Thanks for all the help.  I think using planes and projections are helping.  The attached picture was done in Inventor using Frame Generator.  I love that program!  I'm not sure how I would do it without it. 

 

I have been picking points and using snaps for so long It's hard to figure out how to do anything without them!  But I'll get there.

 

 

Contributor
spsid13
Posts: 19
Registered: ‎09-02-2014
Message 9 of 10 (308 Views)

Re: Moving solids in multi-body parts

09-08-2014 11:32 PM in reply to: killbox

Hi KillBox,

 

Did you finally find a away to move like it happens on autocad with snapping? Even i have recently shifted to inventor 2011 from AutoCad.

*Expert Elite*
JDMather
Posts: 27,601
Registered: ‎04-20-2006
Message 10 of 10 (290 Views)

Re: Moving solids in multi-body parts

09-09-2014 04:10 AM in reply to: spsid13

spsid13 wrote:

Hi KillBox,

 

Did you finally find a away to move like it happens on autocad with snapping? ....


Assembly constraints do the same thing.

Attach your assembly here.

(actually - I recommend you start a new thread as this one has been solved)

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
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Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015-SP1 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
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