Turbine Blade with defined chord/twist at sections

[Anonymous]

Hi,

I am working on a turbine blade, still predesign phase; so chord, twist and airfoil at each section may change frequently. Therefore I want to make flexible enough inventor file so I can change blade easily from parameters. Blade is divided into sections (i.e. 20 sections) along the radius, and each station has predefined chord length and twist. Airfoil at each section is lets say the same for now. All sections are aligned at %25 of their chord and twist is applied from there. I thought that I should create a part for airfoil, assembly for blade and then I can copy the part at each section with scale factor to set chord using as parameter (preferably imported from XML file). So when I change airfoil from the part file, all sections at the assembly will change as well. After all set, finally using loft blade will be created. 

So I've created a spline sketch from airfoil points(see screenshot 1), boundary patched it to create surface, created an assembly, defined planes for sections in assembly file. However I couldn't manage to set chord and twist at each section accordingly. The problem is when I scale the sketch, leading edge point is scaled as well but it should stay at (0,0) and other points should be scaled respect to chord length (see screenshot 1-2-3-4). Additionally, I've created an axis at %25 of the chord so that I can set constrain for all stations at that axis and set twist. But after scaling, its position is wrong as well. (see screenshot 5-6). I've looked at "derive" commend as well with no luck.

After sketching blade, I will use pattern to sketch rotor and will use that for CFD. Because turbine is in still predesign phase, there are many blades to be sketched and simulated. So I can't sketch all blades by hand, It should be automated somehow. I am not a pro Inventor user, however I am using Inventor frequently for 1-1.5 year. Can you guys guide me to solve these problems or is there any similar task experience to be shared? Thanks a lot.

Best regards,
Abdurrahman

[Anonymous]

Hi,

I am working on a turbine blade, still predesign phase; so chord, twist and airfoil at each section may change frequently. Therefore I want to make flexible enough inventor file so I can change blade easily from parameters. Blade is divided into sections (i.e. 20 sections) along the radius, and each station has predefined chord length and twist. Airfoil at each section is lets say the same for now. All sections are aligned at %25 of their chord and twist is applied from there. I thought that I should create a part for airfoil, assembly for blade and then I can copy the part at each section with scale factor to set chord using as parameter (preferably imported from XML file). So when I change airfoil from the part file, all sections at the assembly will change as well. After all set, finally using loft blade will be created. 

So I've created a spline sketch from airfoil points(see screenshot 1), boundary patched it to create surface, created an assembly, defined planes for sections in assembly file. However I couldn't manage to set chord and twist at each section accordingly. The problem is when I scale the sketch, leading edge point is scaled as well but it should stay at (0,0) and other points should be scaled respect to chord length (see screenshot 1-2-3-4). Additionally, I've created an axis at %25 of the chord so that I can set constrain for all stations at that axis and set twist. But after scaling, its position is wrong as well. (see screenshot 5-6). I've looked at "derive" commend as well with no luck.

After sketching blade, I will use pattern to sketch rotor and will use that for CFD. Because turbine is in still predesign phase, there are many blades to be sketched and simulated. So I can't sketch all blades by hand, It should be automated somehow. I am not a pro Inventor user, however I am using Inventor frequently for 1-1.5 year. Can you guys guide me to solve these problems or is there any similar task experience to be shared? Thanks a lot.

Best regards,
Abdurrahman

[johnsonshiue]

Hi! The images are nice but they do not help understand the behavior better. Please attach the part here so forum experts can comment further.

Many thanks!

[johnsonshiue]

Hi! The images are nice but they do not help understand the behavior better. Please attach the part here so forum experts can comment further.

Many thanks!

[Anonymous]

Actually, I didn't upload the part/assembly files since I couldn't manage to set things right and I didn't want to misdirect the people. However, I am attaching the part file. Many thanks.

[Anonymous]

Actually, I didn't upload the part/assembly files since I couldn't manage to set things right and I didn't want to misdirect the people. However, I am attaching the part file. Many thanks.

[johnsonshiue]

Hi! Could you attach s803-spline.ipt also? The assembly needs to load the part.

Many thanks!

[johnsonshiue]

Hi! Could you attach s803-spline.ipt also? The assembly needs to load the part.

Many thanks!

[Anonymous]

It is nothing more that the sketch that used for patch. Thanks again

[Anonymous]

It is nothing more that the sketch that used for patch. Thanks again

[johnsonshiue]

Hi! I think the main problem is the spline in the 2D Sketch. There are a few areas with high curvature. You will not be able to loft it successfully. Also you may want to use two splines instead of one to create the section. The two splines on the leading edge should be G1 (tangent) continuous and ending with G0 continuity at the tail end.

Actually, this is not a very easy task for a beginner. You may need to use Inventor more and understand the workflows better. I don't see a point using Derive Assembly in this case. I am able to use Derive Part and scale the sketch blocks. Please take a look at attached example. Let me know if you have any question.

Many thanks!

[johnsonshiue]

Hi! I think the main problem is the spline in the 2D Sketch. There are a few areas with high curvature. You will not be able to loft it successfully. Also you may want to use two splines instead of one to create the section. The two splines on the leading edge should be G1 (tangent) continuous and ending with G0 continuity at the tail end.

Actually, this is not a very easy task for a beginner. You may need to use Inventor more and understand the workflows better. I don't see a point using Derive Assembly in this case. I am able to use Derive Part and scale the sketch blocks. Please take a look at attached example. Let me know if you have any question.

Many thanks!

[Anonymous]

Hi,
Thanks for your answer I got the main idea and started to search for "Sketch Block" concept. To set chord I can use the scale factor. Is there any wise way to set twist for each section, I mean I need to give angle at %25 chord of that section. Many thanks.

[Anonymous]

Hi,
Thanks for your answer I got the main idea and started to search for "Sketch Block" concept. To set chord I can use the scale factor. Is there any wise way to set twist for each section, I mean I need to give angle at %25 chord of that section. Many thanks.

[johnsonshiue]

Hi! You could probably rotate the sketch block section to get the twist. Or, you use a rail to provide the twist. Please try it out and post what you have. Forum experts should be able to help your further.

Many thanks!

[johnsonshiue]

Hi! You could probably rotate the sketch block section to get the twist. Or, you use a rail to provide the twist. Please try it out and post what you have. Forum experts should be able to help your further.

Many thanks!

[Anonymous]

I've managed to create a blade geometry by deriving a part file that contains sketch of the airfoil by spline and rotating it manually for each section, and using scale factor to set chord just before I've seen your reply about "Sketch block". I liked that function and I am reading about it now, appreciated again. I've started for CFD analysis of this blade. The main problem is this, even I have CAD file of that one blade that I need to analyze, there are many more, and I've created this blade all manually which is a tedious process. I am looking for a wise way that I can change chord and twist by using "Parameters" easily, optionally if I can change airfoil for each section easily somehow, that would be great. So the main problems while I am trying to do this are;

Scaling factor while deriving part file is seen on "Parameters", however when I change that parameter, for example, 1 to 2 (see screenshot 11-12), the sketch doesn't scale, nothing happens. I've tried this as drive from part file that contains sketch and sketch block. While using sketch block, the name of the block changes when I change parameter of scale factor, for example, the block name in the file that you gave me changes from "Block1" to "Block1_2.0x" when I change scale factor from 1 to 2 from "Parameters". However, the sketch doesn't scale up/down either. 

Another thing is I've rotated the sketch to give the twist I want, however I can't set that angle as a parameter. It doesn't show up in "Parameter" section. I've tried many things with no lock, for example, entered angle as "twist = 20.00 deg", however It doesn't accept it(see screenshot 13).

If there is any hint that you can give me, It would be great. Many thanks.

[Anonymous]

I've managed to create a blade geometry by deriving a part file that contains sketch of the airfoil by spline and rotating it manually for each section, and using scale factor to set chord just before I've seen your reply about "Sketch block". I liked that function and I am reading about it now, appreciated again. I've started for CFD analysis of this blade. The main problem is this, even I have CAD file of that one blade that I need to analyze, there are many more, and I've created this blade all manually which is a tedious process. I am looking for a wise way that I can change chord and twist by using "Parameters" easily, optionally if I can change airfoil for each section easily somehow, that would be great. So the main problems while I am trying to do this are;

Scaling factor while deriving part file is seen on "Parameters", however when I change that parameter, for example, 1 to 2 (see screenshot 11-12), the sketch doesn't scale, nothing happens. I've tried this as drive from part file that contains sketch and sketch block. While using sketch block, the name of the block changes when I change parameter of scale factor, for example, the block name in the file that you gave me changes from "Block1" to "Block1_2.0x" when I change scale factor from 1 to 2 from "Parameters". However, the sketch doesn't scale up/down either. 

Another thing is I've rotated the sketch to give the twist I want, however I can't set that angle as a parameter. It doesn't show up in "Parameter" section. I've tried many things with no lock, for example, entered angle as "twist = 20.00 deg", however It doesn't accept it(see screenshot 13).

If there is any hint that you can give me, It would be great. Many thanks.

[johnsonshiue]

Hi! The behavior sounds like a bug to me. It should work. Could you attach the files exhibiting the behavior?

Many thanks!

[johnsonshiue]

Hi! The behavior sounds like a bug to me. It should work. Could you attach the files exhibiting the behavior?

Many thanks!

[Anonymous]

Hi,
I've tried this on the file that you shared in 6th post of this topic. I am adding the files anyway. Many thanks.

[Anonymous]

Hi,
I've tried this on the file that you shared in 6th post of this topic. I am adding the files anyway. Many thanks.

[johnsonshiue · Accepted solution]

Hi! I think I see the issue. After you change the scale parameter, you will need to edit the first derive node -> hit Ok so the change becomes effective. Regarding rotating the sketch block, it seems to work fine for me. Please take a look at attached files.

I guess you thought sketch rotation is parametric. But, it is not parametric. The rotate angle is just a angular value, which does not create a new model parameter. You will need to create a new dimension or a constraint to lock it in the place.

Many thanks!

[johnsonshiue · Accepted solution]

Hi! I think I see the issue. After you change the scale parameter, you will need to edit the first derive node -> hit Ok so the change becomes effective. Regarding rotating the sketch block, it seems to work fine for me. Please take a look at attached files.

I guess you thought sketch rotation is parametric. But, it is not parametric. The rotate angle is just a angular value, which does not create a new model parameter. You will need to create a new dimension or a constraint to lock it in the place.

Many thanks!

[Anonymous]

Hello,

I also have a problem, when I want to loft all of the airfoil sections. Can you please look at the attached pictures and see what is the problem. 

[Anonymous]

Hello,

I also have a problem, when I want to loft all of the airfoil sections. Can you please look at the attached pictures and see what is the problem. 

[johnsonshiue]

Hi! I cannot make much sense out of the picture. Could you attach the file here or send it to me directly (johnson.shiue@autodesk.com)?

Many thanks!

[johnsonshiue]

Hi! I cannot make much sense out of the picture. Could you attach the file here or send it to me directly (johnson.shiue@autodesk.com)?

Many thanks!

[Anonymous]

Thank you for your time. I've just sent it to you.

[Anonymous]

Thank you for your time. I've just sent it to you.

[Anonymous]

Thank you I figured out how to fix it. I changed the transition of automatic mapping in loft and fix it.

[Anonymous]

Thank you I figured out how to fix it. I changed the transition of automatic mapping in loft and fix it.

[johnsonshiue]

Hi Katie,

Many thanks for sharing the file with me! I have replied to you via email about the same thing. You just need to uncheck Automatic Mapping and select the end of the foils. Also, make sure "Merge tangent faces" option is checked. It will create a nice smooth surface with fewer edges.

Thanks again!

[johnsonshiue]

Hi Katie,

Many thanks for sharing the file with me! I have replied to you via email about the same thing. You just need to uncheck Automatic Mapping and select the end of the foils. Also, make sure "Merge tangent faces" option is checked. It will create a nice smooth surface with fewer edges.

Thanks again!