Inventor: Sketch problem

[Anonymous]

Hi,

I am new to this forum. Learning Inventor 2016. I am trying to draw a simple screw thread. I have drawn the first thread which "revolves" nicely. But when I copy the same thread again, the inventor doesn't pick the complete sketch in the revolve command, It only selects half of the sketch. I am very puzzled as I have spent a lot of time figuring what is happening here. But still no idea.

I have attached 2 screen shots here. One is the sketch itself. And other shows that revolve command (not the white portion of the sketch, showing that it is selecting half the sketch only).

Any help is appreciated. Thanks.

[Thomas_Savage]

Hello,

Could you attach your part file?

It could be because where the lines meet it is not constrained. That is why it doesn't pick it all up.

Check they are constrained.

Or reconstrain them with coincident constraint.

Hope this helps?

Thomas.

[Anonymous]

Hi,

Thanks for your quick reply. I tried adding coincident constraint, but it would not let me. See attached file.

Regards

[TheCADWhisperer]

Revolve will never result in a helical thread.

Do it the same way that you do it out on the shop floor.

Create a cylinder (you can do this with Revolve or Extrude).

Sketch triangle for single point cutting tool.

Use the Coil command to cut the helical thread.

You should never have Zero (0) length dimensions - use Coincident instead.

You should not have repeated dimensions - use Equal (=) instead.

Do not use dimensions that cannot be inspected (generally beyond 2 or 3 decimal places).

[Anonymous]

I know what you are saying about the helical thread. I am preparing this sketch/model for a 2D stress analysis in Ansys. However I will look at the other points you have mentioned.

Thanks for your reply.

[Thomas_Savage]

I have attached a part file to show you the coil. And how it cuts the profile around the cylinder. So you can see how it works.

Hope this helps.

Thomas.

[TheCADWhisperer]

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@Anonymous wrote:

.... I am preparing this sketch/model for a 2D stress analysis in Ansys. ...

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Pattern features - not sketch elements.

[johnsonshiue · Accepted solution]

Hi! @TheCADWhisperer is right. Dimensions should be placed for inspection purpose. They should not be placed just for the sake of being fully-constrained. I suspect you use Auto-Dimension command to do that without properly constrain and dimension first. Auto-Dimension command works best when you have properly dimensioned geometry imported from another CAD system. Auto-Dim helps you save the time to recreate the relationship. However, it still can establish the wrong relationship. You need to look at each dimension and make sure it is sensible.

To make this case work, you need to delete those dimensions created by Auto-Dimension. Then right-click on the sketch icon in the browser -> Sketch Doctor. You will see there are three places causing the loop to be open. Select the proper segment to close the loop. Then the profile will be closed and revolve should work. If you still cannot figure out, you could delete it and recreate it. It should not be too difficult.

Many thanks!

[Anonymous]

Thanks for all of your replies guys. You have been very helpful.