Need help with creating 45 degree involute spline using Design Accelerator. I trying to create an ANSI B92.1 - 45 Deg., Fillet Root, Side Fit 24/48 - Class 5 involute spline. I created my shaft part with my shaft O.D. at the Major Dia. of 1.167". I created my hub part with an I.D. Minor Dia. of 1.100. I created an assembly and constrained the parts along the shaft axis. but when I go to create spline I get error. "Modeling: Cannot create iFeature!" and "Modeling: Not possible to create shaft groove" I am not new to Design Accelerator and have successfully created several involute splines but have noticed some spline designations give errors when generating. We are using Inventor 2013. I have attached the part and assembly files. Any help would greatly be appreciated. Thank You !
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Regarding to your requirement,I tried on your dataset and got the result as below image.
Have you set orientation of the shaft groove? You will get error message if you don't set orientation, just like you described.
Thank you for the reply Jingyi. I have tried setting the orientation planes. On the shaft part, I set the orientation plane at the YZ plane and on the hub part I selected the XZ plane. Usually, I don't have to physically select them because Inventor does that automatically and spline usually generates. I have also tried changing the way I have it contrained but still made no difference. Currently I have a flush constraint between the two parts at the YZ plane.
Well I got it to work by selecting the orientation of each part along the XZ plane but am baffled as to why that works in that orientation but not YZ plane. When I select the orientation of each part along YZ plane, I get the errors. So this leaves me with more questions:
Is this my path forward by selecting orientation planes at XZ ? In past , I always let Inventor decide because I always constrain the YZ with a Flush constraint and a Mate constraint with the Z axis..
Why does the same process I have always followed work on some splines and not others ?
All parts that I create always rotate along the Z axis, so it would be a modeling error between the differences.
But if it works then I learned to always use the XZ plane as orientation.
Thank You !
YZ plane is not the root of the failure, in this case, you still can use the default YZ plane if you edit its rotation angle by 180 degree.
Since the Involute spline is a ifeature indeed, and iFeature result will be impacted by its position and orientation. I thought it's a preview issue, it doesn't reflect the real modeling result. I have logged it as an issue in tracking system. So far, I still recommended you to pay attention to its orientation when you get error message.
To continue with this discussion, I guess that would make sense as to why it works sometimes and at other times it does not as in this case. For the times it works, is probably due to the fact I have an even number of teeth, therefor the angle of rotation of YZ plane would not matter 0° vs.180°. In this case it does because of odd number of teeth. This is what seems logical to me anyway, is this correct? It will not generate due to not having teeth aligned. I guess I always thought Inventor was smart enough to decypher that you would want the teeth of a spline aligned.
It shows the preview but will not generate. Thanks for clarifying