topic Re: Cannot Extrude Sketch in Inventor Forum

Cannot Extrude Sketch

Vagulus — Sun, 09 Sep 2018 01:23:42 GMT

I cannot extrude these two hold-down lugs

It's a new sketch, all loops closed, fully constrained. The lugs just won't extrude.

Can someone please explain why?

Thanks

Re: Cannot Extrude Sketch

IgorMir — Sun, 09 Sep 2018 03:01:05 GMT

Hi Vagulus,

It is something in the way you have modeled it. I have changed the model slightly and it works.

Please see the attached.

Cheers,

Igor.

@Vagulus wrote:

I cannot extrude these two hold-down lugs

It's a new sketch, all loops closed, fully constrained. The lugs just won't extrude.

Can someone please explain why?

Thanks

Re: Cannot Extrude Sketch

Vagulus — Sun, 09 Sep 2018 08:28:28 GMT

Thanks Igor. I still couldn't get it to extrude. Used yours .

Re: Cannot Extrude Sketch

IgorMir — Sun, 09 Sep 2018 08:33:56 GMT

It is probably a random glitch in the file. By modifying the sketch for lags in the original file I couldn't get it extruded either.

Cheers,

Igor.

@Vagulus wrote:

Thanks Igor. I still couldn't get it to extrude. Used yours .

Re: Cannot Extrude Sketch

johnsonshiue — Sun, 09 Sep 2018 14:37:33 GMT

Hi! I took a quick look at the part. This is about profile recognition. There is overlapped sketch geometry. Edit the sketch and delete the Projected Loop in the browser, you will see there are still sketch lines. This kind of condition is not desirable. It can create sloppy model geometry. Please make sure there is no overlapped geometry.

Many thanks!

Re: Cannot Extrude Sketch

Vagulus — Sun, 09 Sep 2018 23:27:26 GMT

@johnsonshiue wrote:
Edit the sketch and delete the Projected Loop in the browser, you will see there are still sketch lines. This kind of condition is not desirable. It can create sloppy model geometry. Please make sure there is no overlapped geometry.
My procedure was (or should have been) to project the geometry, convert the projected lines to construction lines, then overdraw the construction lines. Does the conversion to construction lines not remove the overlapped geometry problem?

Re: Cannot Extrude Sketch

IgorMir — Mon, 10 Sep 2018 01:23:57 GMT

Hi Johnson;

When I was working on the model - I have completely removed that sketch and created a new one. On one side only. The profile was extrudable, but the Mirror of that lag afterwards - failed. Than I tried to introduce the similar sketch on the other side. The extrusion for both profiles failed all together. Once I have modified the main body (I have used Shell instead of Thicken) - creating of lags wasn't a problem. What do you think of that?

Cheers,

Igor.

@johnsonshiue wrote:

Hi! I took a quick look at the part. This is about profile recognition. There is overlapped sketch geometry. Edit the sketch and delete the Projected Loop in the browser, you will see there are still sketch lines. This kind of condition is not desirable. It can create sloppy model geometry. Please make sure there is no overlapped geometry.

Many thanks!

Re: Cannot Extrude Sketch

IgorMir — Mon, 10 Sep 2018 01:23:11 GMT

In your particular case - there is no need to project the whole geometry. Projecting two corner points is more then enough. After that - draw a rectangle and constrain two corners of it to corresponding points. You will need only one dimension to specify the length of the lag and the sketch will be fully constrained.

Cheers,

Igor.

@Vagulus wrote:

@johnsonshiue wrote:

Edit the sketch and delete the Projected Loop in the browser, you will see there are still sketch lines. This kind of condition is not desirable. It can create sloppy model geometry. Please make sure there is no overlapped geometry.

My procedure was (or should have been) to project the geometry, convert the projected lines to construction lines, then overdraw the construction lines. Does the conversion to construction lines not remove the overlapped geometry problem?

Re: Cannot Extrude Sketch

johnsonshiue — Mon, 10 Sep 2018 01:24:36 GMT

Hi Igor,

Currently, Inventor sketch profile recognition is based on constraints. The reason why mirror or pattern of sketch geometry does not constitute profiles is because lack of coincident constraints. This limitation has been there since day 1. It is very annoying and it makes sketching very difficult to use. Also, it increases the need to create overlapped sketch geometry unnecessarily. The sketch becomes very messy easily.

We have been investigating how to recognize profiles purely based on geometry. If there is a solution, it will be for new release, not for existing releases.

Many thanks!

Re: Cannot Extrude Sketch

IgorMir — Mon, 10 Sep 2018 01:36:18 GMT

Hi Johnson,

I can't really say I follow you. In the model I have posted to the OP - everything works - as expected. But I do agree that the sketches should be made as simple as possible. That's what OP will learn soon, I hope.

Cheers,

Igor.

@johnsonshiue wrote:

Hi Igor,

Currently, Inventor sketch profile recognition is based on constraints. The reason why mirror or pattern of sketch geometry does not constitute profiles is because lack of coincident constraints. This limitation has been there since day 1. It is very annoying and it makes sketching very difficult to use. Also, it increases the need to create overlapped sketch geometry unnecessarily. The sketch becomes very messy easily.

We have been investigating how to recognize profiles purely based on geometry. If there is a solution, it will be for new release, not for existing releases.

Many thanks!