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Copying spline to a new work plane and linking to the original.

17 REPLIES 17
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Message 1 of 18
ghulands
2078 Views, 17 Replies

Copying spline to a new work plane and linking to the original.

Hi,

I am new to Inventor and 3D modelling. I have gone through the three tutorials that comes with Inventor on modelling a part. I am now trying to model a fuselage for an RC plane and am trying to copy a spline from one work plane to a new one and link them together so that if I edit one, it is reflected in the other. Copying and then pasting into the new plane doesn't link the two splines together.

 

If anyone can point me in the right direction would be greatly appreciated.

 

Cheers,
Greg

 

fuse.png

17 REPLIES 17
Message 2 of 18
CCarreiras
in reply to: ghulands

Hi!

 

Start a new Sketch in the new plane and use the "Project geometry" tool and pick the geometry from the first sketch to transport that geometry for the new sketch.

 

Regards.



Regards.
CCarreiras
Message 3 of 18
JDMather
in reply to: ghulands

You will need to dimension (parametric) the sketches to link them together so that one can have dimensions as functions of another.

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

 

otherwise Project Geometry if the dimensions aren't going to be different between the two sketches.

But if the dimensions aren't going to be different - why would the second sketch be needed?

 


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Message 4 of 18
ghulands
in reply to: JDMather

Thanks for the link to the PDF JDMather.

 

I should probably tell you my end goal as I may be using an inappropriate technique. Once I have the model of the fuselage, I plan to get it CNC'd out of foam a couple of mm smaller than the modelled size so I can then fiberglass it a little oversize. Then I will get it CNC'd to size. Then I will make the fiberglass molds from the plug.

 

I thought the right approach would be to create the "ribs" along the Z axis and then loft them together. When selecting the planes in a single loft, it balloons the fuselage.

 loft one step.png

 

When I loft it in 2 discrete steps, I loose a nice blending between the two.

 

loft 2 steps.png

 

Am I taking the right approach for my end goal? The other approach I have thought about is making splines along the Z axis (the length of the fuselage) to make "stringers" and then make surface from there.

 

Thanks for the help,

Greg

Message 5 of 18
JDMather
in reply to: ghulands


ghulands wrote:

 .... When selecting the planes in a single loft, it balloons the fuselage.

 

Greg


Create Guide Rails for absolute control.
I recommend you do my Vacuum tutorial.

 

http://home.pct.edu/~jmather/content/DSG322/Inventor%20Tutorials/Inventor%202011%20Tutorial%2014.pdf


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Message 6 of 18
ghulands
in reply to: JDMather

Thanks for the quick reply. I think it might be best if I do all your tutorials 🙂

 

Cheers,

Greg

Message 7 of 18
JDMather
in reply to: ghulands

http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm

 

Unfortunately most of them are rather old now.


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Message 8 of 18
ghulands
in reply to: JDMather

I'm sure the concepts still apply, maybe just the way to do it is slightly different?

Message 9 of 18
JDMather
in reply to: ghulands

All should still work (there is a problem in the "horseshoe" sketch in the test instrument file, I don't recall if I fixed it).

 

But there are a lot of new tools that didn't exist back then.

The Vacuum tutorial is fairly recent and has some simularity to your current design.


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Message 10 of 18
ghulands
in reply to: JDMather

I finally had some time to work through the tutorials and then have another go at what I was trying to achieve. I created a nose plane, then put the main cross section on the next plane. I then projected the geometry on the next 4 sections and made the last section have a circle for rear of the fuselage. I used splines for the rails in a 3D sketch.

 

When lofting now, if i select all the sketches and rails I get an error saying that one or more of the rail curves doesn't intersect one or more sections.loft_all_sections_selected.png

 

If I change the loft to be from the first section and to the last section without selecting the intermediate sections, The loft ends up with waves between the rails.

 

loft_first_n_last_with_rails.png

 

Looking side on to the rails, you can see that because I used splines that the curve doesn't go to the sketch on the cross sectional sketches. However, I anchor the spline to the points on the sketch.

 

rails_cross_section.png

 

To satisfy the error when doing the loft, is the right process to then project the rail geometry back to the sketches and create a "bulk head" using the those points?

 

Thanks in advance for any guidance,

Greg

Message 11 of 18
JDMather
in reply to: ghulands

Attach your ipt file here.

You should be able to edit sketches to correct missing connections.


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Message 12 of 18
ghulands
in reply to: JDMather

Attached.

 

Thanks,
Greg

 

Message 13 of 18
JDMather
in reply to: ghulands

You are doing too much work.

You have 5 repeated sketches - these are not needed.

Your 3Dsketch is actually 2D, therefore I would do it as a 2D sketch.

 

I'll post my solution tomorrow.


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Message 14 of 18
CAG_DRAFT
in reply to: JDMather

I'm quite interested to see this, I've got a few issues with getting lofted surfaces to do exactly what I want.

Hopefully the solution JD posts is a 2013 file...

Message 15 of 18
JDMather
in reply to: CAG_DRAFT


@CAG_DRAFT wrote:

I'm quite interested to see this, I've got a few issues with getting lofted surfaces to do exactly what I want.

Hopefully the solution JD posts is a 2013 file...


There is no one single solution for every Loft problem.

Since there were very few dimensions on the posted part - I made up my own interpretation (see attached file).

 

Notice that there are no extra workplanes and only two simple 2D sketches.

 

I recommend reading this document - particularly the section on fully constraining sketches.

http://home.pct.edu/~jmather/skillsusa%20university.pdf

 


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Message 16 of 18
ghulands
in reply to: JDMather

Hi JD,

Thanks so much for doing that. I think my problem boils down to three things

 

  1. Not knowing the best way to break down the final geometry I was after into a minimalist form.
  2. Not knowing the best sequence of commands to achieve the final geometry. Is there a rule of thumb in Inventor like arthimetic operator precedence (eg. multiple before addition)?
  3. Good 2D sketching skills. Along with doing the tutorials on your site, I also bought the Learning Autodesk Inventor 2014 DVD which did help me a lot from when I first tried to sketch the fuselage. That DVD also made clear that having a fully constrained sketch is important.

I just went back to my sketch to try to constrain the the main fuselage shape and was still not able to, so I just wanted to ask a couple of questions on how you did that sketch. Did you create half of the sketch and then mirror it (I know you recommend against mirroring but not sure if mirroring a spline is an acceptable use of it)? What is the significance of the points down the center line? What does placing a work point on the XY plane help with?

 

For sketch 2, was the reason you dimensioned it with the diametral dimension and depth, instead of dimensioning to the arc point (like you did on the arc marked 600) because you knew you were going to revolve the nose?

 

I think as I use the application more I will get more fluent on the 2d sketching, and a better understanding of the interaction of operations to better sequence the commands to achieve the final geometry in the least amount of steps. At the moment I think learning the rationale behind why you did certain things will go a long way to help the later one.

 

Thanks again for your help, JD, I really appreciate it.

 

Greg.

Message 17 of 18
JDMather
in reply to: ghulands

The first identification of geometry was easy.

If the profile doesn't change - then Extrude the feature.  Only one sketch needed.

 

More or less -

Extrude or Revolve, Hole, Fillet, Chamfer (Fillets and Chamfers as late as possible).
Sweep, Shell

Loft

Bend Part

Surface modeling

...but not hard and fast rules.  Often (quite often) I will start out with surface modeling simply becuase it is the shortest, least amout of work towards the finish.  Many think they have no need for surface modeling becuase they don't do curvy, organic shapes.  I have a collection of examples of simple geometry parts that are just easier to complete starting out with surfaces.

 

Mirror of sketch points in this problem would have been just as good as what I did.

I created a bunch of horizontal construction lines out in space and then added Coincident Midpoint constraints to constrain to the vertical line - the same as mirroring points.  DO NOT in most cases) mirror a spline.

 

The workpoint was to define the pierce location of the spline and the YZ plane. If you zoom in on that location you will see that the construction geometry and the spline intersect the YZ plane at slightly different locations because a Control Vertex Spline was used rather than an Interpolation Spline.  If an Interpolation Spline had been used - the Work Point1 would not have been needed.  It is coincident that the workpoint also appears on the XY plane (because the 2D sketch spline is on the XY plane.  The significance is the pierce of the YZ plane of the spline at that point.  That gives me a point to connect the Rail in Sketch2.

 

The diametral dimensions could have been dimensioned as radii, but when creating 2D drawings from the model - I can Retrieve the diametrals which I probably want in the 2D documentation.

 

Practice, practice, practice and get lazy - do a part and then do it again using what you learned from first attempt to simplify.  Over time you will learn to simplify from the start and realize you were doing too much work in the past.  Get lazy.  Figure out the easy way to aviod work. 

 

I'm sure if I re-did this part I could simplify my initial attempt - I did too much work on Sketch2.  I did too much work on Sketch1 - it would have been fewer clicks to create the points and mirror rather than add midpoint constraints to a bunch of construction lines.  But when I did Sketch1 I was still trying to figure out your design intent.

 

It is often better to loft between solid and/or surfaces rather than sketches - as there are more options for control.
If I remember - tomorrow I will post a link from an AU 2012 presentation which is very good for understanding how Inventor creates your geometry.

 

 

  


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Message 18 of 18
ghulands
in reply to: JDMather

Thanks for some insight into your process - it helps a lot.

 

I started to model a servo the other night and it doesn't look too bad - but it definitely could be a lot simpler. That will be this weekends task. And then I'll take another stab at the fuselage.

 

Thanks for all your help.

 

Cheers,

Greg

 

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