Derived sketches - copy sketch across to different plane

[Anonymous]

Hi all,

Is there a way to get a derived sketch going similar to the method in Solidworks? Where you can insert a derived sketch into a new plane inside the same part.

This is a hugely important feature, I need to do a lot of lofting with complicated rails, and I need to get the rails exactly the same across a few sides of the profile. These rails aren't arcs, they're usually splines. The parts are very organic so I can't use any form of duplicating body sections and combining them.

I know there is a copy paste feature for sketches across planes, but they lose relationships, so when I edit the first rail, it doesn't modify the rest.

If anyone has any solutions, please let me know.

Thanks!

[torbjorn_heglum1 · Accepted solution]

Have you looked into sketch blocks?

A sketch block can be used several times in different sketches within one part, and if required, also derived to another part.  If you change something inside the block, all instances will update accordingly.

Torbjørn  

[johnsonshiue]

Hi! I believe you want to look into Sketch Block workflows. Regarding source sketch, is there any projected geometry? Or, it contains only the regular sketch geometry?

Many thanks!

[Anonymous]

Hello, I can't project geometry because the work planes are at various angles. 

I will check into sketch blocks today and see how it goes !

[Anonymous]

Hi !

Thank you, that worked ! I've been copy pasting the blocks across planes and they have been keeping their relations, which is great. 

Only thing I want to figure out is how to stop it from rotating when I paste a block into a new plane. I have to keep re-orienting every block so far. Is there a solution for this ?

Apart from that, it's totally fine!

[torbjorn_heglum1]

Inventor auto-selects coordinate system when a sketch is created. I don't know any way to change settings for this, so I guess you will have to keep rotating the blocks.

Torbjørn

[SBix26]

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@Anonymous wrote:

Only thing I want to figure out is how to stop it from rotating when I paste a block into a new plane. I have to keep re-orienting every block so far. Is there a solution for this ?

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Sketch blocks should be constrained properly no matter what, so it's probably a good reminder for you that they are initially placed "disoriented".

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Sam B
Inventor Pro 2019.3 | Windows 7 SP1
LinkedIn

[jimmyflash]

As I found the Derived Sketch feature in SolidWorks today I was amazed, how great is works and how simply can be the sketch cloned to any location in the same model.

How it works? Simply select the Sketch and the Plane and execute the feature. Now is just needed to constrain entire sketch in new location.

Unfortunately Sketch Blocks are really limited feature to be used as a equivalent tool to SW Derived Sketch. When in blocks is no way to use Projected Geometry it is a dead end and is not necessary to try to use the blocks anymore. It is useless.

I believe the Derived Sketch could bring new huge advantage to all of us.

[johnsonshiue]

Hi Jimmy,

When you said Inventor Sketch Block does not allow projected sketch, it is true that the sketch block itself does not allow it. It is because the project source geometry may not be available. You can still project it but you will need remove the project constraint in order to include the geometry in a sketch block.

The sketch that contains a sketch block still allows projection. I am a bit curious about the usage. If possible, please share a workflow or a video showing the behavior in SWX.

Many thanks!

[jimmyflash]

Hi John,

when you said "you will need remove the project constraint" it is not projected anymore and loosing the benefit of projection usage. It is really useless. Blocks are good for some standardized library shapes or labels.

Here is the video how it works in SW:

https://www.youtube.com/watch?v=SptORejXdec&ab_channel=InnovaSystems-ExpertsinSOLIDWORKSTraining%26S...

There is the huge amount of better usage of Derived Sketches than parralel copy to create the same size key slot of course. Really complicated sketches could be by a few clicks duplicated to surface with absolutely different oriantation.

To copy sketch and set multiple dimensions to be related to original sketch is not needed anymore.

Just simple and amazing!

Sketching is the basic operation and everything starts here. Such huge improvement here is essential.

Of course the link could be broken anytime.

Another videos:

https://www.youtube.com/watch?v=aYn0PXruhNw&ab_channel=TriMech

https://www.youtube.com/watch?v=3kTnAHvW7M4

[johnsonshiue]

Hi Jimmy,

Many thanks for sharing the videos! I have to say the workflow is pretty slick. Sketch Block is similar but not the same. But, I fail to understand what was happening at 1:39. What was the constraint? The profile actually rotates a bit.

[jimmyflash]

Yes, perpendicular constraint.

[johnsonshiue]

Hi! Then I would argue that it is also doable in sketch block. You need to project the edge from the other hexagon hole. Then apply the perpendicular constraint.

[jimmyflash]

It is worthless to try to look for solution with sketch blocks.

You found the way to constrain the block, but the most of sketches are dependent on projected geometry, so you have nothing to be constrained, when you are not able to create the original sketch.

Forget on hexagon and think about really komplex sketches.

[johnsonshiue]

Hi! I guess I did not fully digest the power of SWX derived sketch. Just purely based on the video, I am not seeing the ability to include projected geometry in the derived sketch. The two sketch planes are parallel and the geometry can be projected to the sketch without a problem. What if the target face isn't on a parallel plane?

I am not a SWX expert, though I do use it from time to time. Please feel free to try it on a more complicated case and see how it works.

Many thanks!

[robert.gephart]

Hello Johnson and all,

I have worked SW and Inventor but wondered why I had to search for this for Inventor that seems so basic and powerful in SolidWorks. That video only scratched the surface on the uses for derived sketches.

Just another mention for this for Autodesk to make this happen in Inventor. Also, the sketch environment is way powerful in SW.

[Frederick_Law]

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@robert.gephart wrote:

Hello Johnson and all,

I have worked SW and Inventor but wondered why I had to search for this for Inventor that seems so basic and powerful in SolidWorks. That video only scratched the surface on the uses for derived sketches.

Just another mention for this for Autodesk to make this happen in Inventor. Also, the sketch environment is way powerful in SW.

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Just want to say equation is so basic in IV but it doesn't work 100% in SW.

SW don't have time to fix it but they list which won't work in help.

Now it depends on why I need to "copy" a sketch.

iFeature is one way to "copy" a sketch in IV.

Got example of how and why you need derive sketch in same part?

[johnsonshiue]

Hi Robert,

The ability to relocate derived objects is indeed limited. For solid bodies and surface bodies, you may use Move Bodies command (or Direct Edit for solid bodies). But, for sketch, relocation isn't possible. One thing you may consider is to leverage sketch blocks workflows. For shapes that you may reuse repeatedly, you can create sketch blocks (in 2D sketch panel -> right-click on the ribbon -> Show Panels -> check Layout). You can copy and paste sketch blocks between sketches and between files. Also you can derive them into new parts. A sketch block is a 2D rigid body which can be placed on any 2D sketch.

Many thanks!

[armansesar]

Sketch Blocks work great for inserting small repeated geometries within the same sketch or within the same part or even across multiple files, but derived sketch function is an absolutely necessary tool for complex sketches. This is one of the main issues I have come across designing in Inventor. One good scenario is for having an identical sketch duplicated across multiple planes angled along a central axis typically seen in radial parts. Think of designing a cup and a lid. The cup is one part or one body revolved from an original sketch drawn on for example XY (front) plane, while the lid geometry is designed in another file, or within the same file, in a separate sketch with projected geometry from the main cup sketch also on XY plane. So far so good, because you can do this on the same plane whether you are in the same file or a secondary file. But, now imagine you are adding a spout to the cup, but the spout must be at a 30 degree angle from the original XY plane. Currently, the only way to do this (not including direct edit) is to create the appropriate plane and have your spout geometry reference projected cut edges from the solid body you are working from. If a solid body does not exist, you must create a solid body or surfaces to reference for this purpose alone, and unfortunately, projected cut edges often lose reference and must be re-projected if any modifications are made upstream that alter the shape or ID of the particular face...etc, and subsequently any features such as extrudes or revolves relying on these sketches will also need to be corrected once projected cut edges are lost and re-projected.

This is a huge hassle for complex parts and complex features. Not to dive into issues with projecting cut edges, since projecting cut edges individually are sometimes allowed and sometimes impossible, and projecting cut edges function projects all cut edges at once which is often unnecessary and confusing, and if one projection constraint is deleted, all edges lose reference constraints and must be deleted and reprojected in order to access the few edges you require.

Unfortunately direct edit is also not a very intuitive or recommended work flow for designing features but more of a last resort shortcut for modifying features. 

[johnsonshiue]

Hi! Many thanks for the detail explanation! I think I understand your request. Let me borrowing your cup and lid example. If the cup is a revolution of a 2D sketch block, you may place the same sketch block on a different plane (rotated 30 degree from the origin plane). Then there is no need to do project cut edges.

Regarding project cut edges losing associativity, it sounds like a bug to me. Please share an example that exhibits the behavior. I would like to understand it better.

Thanks again!