Moving sketch plane

[Maavhamt]

Hi,
I created a sheet metal part then added flanges at either end by drawing on the bottom surface of the object then using "Tab". Since then I lowered the bottom surface of the object by 10mm. I have found the flanges stayed where they where because the sketch plane hasn't moved. Is there a way to get the sketch plane to follow the bottom surface of the object, or do I have to redraw the flanges?

 

[batejosh]

You can't change sketch planes after you've made a drawing. The only way is to draw a sketch on its own new plane and you can modify that plane later if you want.

The best workaround I find is to copy and paste ('Ctrl'+'T') the sketch figures from the old sketch. Can sometimes save time. You still need to do an amount of re-constraining.

 

[Ralf]

You can't change sketch planes after you've made a drawing. The only way is to draw a sketch on its own new plane and you can modify that plane later if you want.

The best workaround I find is to copy and paste ('Ctrl'+'T') the sketch figures from the old sketch. Can sometimes save time. You still need to do an amount of re-constraining.

You can use an existing 2D Sketch and project this 2D Sketch with "Project to Sketch" onto a new plane.

Just a hint:
Drawings are 2D Drawings, but not 2D Sketches in a 3D Part.

 

[batejosh]

Good points all around Ralf! Thanks for the pro-tips. Will have to project to sketch next time

 

[MikeHenry]

You can't change sketch planes after you've made a drawing. The only way is to draw a sketch on its own new plane and you can modify that plane later if you want.

Seems to me that one should be able to change a sketch plane no matter where it was sourced. The lack has often been problematic for me.

 

[batejosh]

Totally agree Mike! Was the second frustrating lack of feature I noticed about Alibre. The first was not being able to insert a mid-plane. I now overcome that by inserting a mid-point (you can do it with points, but not planes), and inserting a plane at that point.

 

[JST]

Seems that there is another level of problem with changing the sketch plane.

The extrusion of the feature which the sketch defines is based on the sketch plane. So if you change the plane, you change the origin of the feature.

While that may be exactly why you want to change planes, it seems as if it is messing with a rather basic portion of the part.... The workarounds of projecting to a different plane will actually get rid of the original sketch, and re-create the feature using what is really a different sketch, which therefore creates a different feature.

It seems that there is a bit of difference between creating a different new feature (even if it is the same feature recreated from a different sketch), vs moving the origin of an existing feature that was originally sketched and based on one of the three original planes.

If the sketch was on a separately defined plane, the definition of the plane is part of the feature, and can be changed, where an original plane (X-Y, Y-Z etc) is a fixed reference that is harder to change.

 

[HaroldL]

The first was not being able to insert a mid-plane.

I've turned in an enhancement request about that.

 

[HaroldL]

Hi,
I created a sheet metal part then added flanges at either end by drawing on the bottom surface of the object then using "Tab". Since then I lowered the bottom surface of the object by 10mm. I have found the flanges stayed where they where because the sketch plane hasn't moved. Is there a way to get the sketch plane to follow the bottom surface of the object, or do I have to redraw the flanges?
View attachment 26527
View attachment 26526

Did you in fact create a plane to sketch the flanges on or, as you stated, sketched on the bottom surface of the object? I'll submit that if you sketched on the bottom surface the sketch plane did move because the surface is your sketch plane. Did you constrain the sketch to the edge of the object?

I just ran a quick test on a sheet metal part, added a Tab flange, and then change the size of the part, both in length and depth. In both instances the Tab followed the edge and part surface it was sketched on simply because I placed a Collinear constraint between the base line of the tab and the edge of the part.

If you created a Plane to sketch the tab on you could possibly "tie" the plane to your object by using the Equation Editor and linking the offset location of the plane to the end or surface of the part.

 

[MikeHenry]

Seems that there is another level of problem with changing the sketch plane.

The extrusion of the feature which the sketch defines is based on the sketch plane. So if you change the plane, you change the origin of the feature.

While that may be exactly why you want to change planes, it seems as if it is messing with a rather basic portion of the part.... The workarounds of projecting to a different plane will actually get rid of the original sketch, and re-create the feature using what is really a different sketch, which therefore creates a different feature.

The other CAD program I use allows one to change the sketch plane and it has never been a problem for me. That's not to say it wouldn't be for someone else. In cases like this, it would really be nice to get some input from Alibre on what sort of problems that implementation of this "enhancement" may cause.

 

[Maavhamt]

Did you in fact create a plane to sketch the flanges on or, as you stated, sketched on the bottom surface of the object? I'll submit that if you sketched on the bottom surface the sketch plane did move because the surface is your sketch plane. Did you constrain the sketch to the edge of the object?

TBH I can't remember. I couldn't find the plane the sketch is on in feature explorer so I don't think I defined a plane for it. As I can't find it I can't change its position. In the end I redrew the sketch on the lower surface. So perhaps in future I should follow your advice and create a plane that is mapped onto the surface so I can move the plane if I need to. It's just that at the time I didn't envisage having to move it.

 

[JST]

If you did not define one, it will be one of the basic 3 planes.

"did not envisage having to move it"....... The most common issue with "parametric" 3D CAD..... and the reason for the "best practices", even though in 95% + of cases they just make more useless work. It's that 5% (or less) that tends to pay handsomely for the extra "useless work" on all the others.

That said, I do not always use the "best practice", and I suspect even the committed preachers of "best practice" also do not ALWAYS use it.

 

[bigseb]

Been touched on many times before: always create proper reference datums! Yes, maybe its a schlepp. maybe its not necessary all the time. But when you need it you gonna be glad its there.

 

[HaroldL]

TBH I can't remember. I couldn't find the plane the sketch is on in feature explorer so I don't think I defined a plane for it. As I can't find it I can't change its position. In the end I redrew the sketch on the lower surface. So perhaps in future I should follow your advice and create a plane that is mapped onto the surface so I can move the plane if I need to. It's just that at the time I didn't envisage having to move it.

While creating sketch planes will help when a hole, cutout or other feature needs to be moved from one plane orientation to another, like from the bottom of a part to the side, I don't necessarily buy into the fact that they are needed when adding flanges or tabs to sheet metal. The reason is that the plane can only track model changes perpendicular to the plane.

I hope you don't mind but I borrowed your image to illustrate:


With a properly constrained sketch the tab, or in your case a flange, will follow a change in both axis shown in the image.

When you are adding holes or cutouts then a properly set up sketch plane will allow you to move them from one surface to an adjacent or other surface by changing the orientation angle or offset of the plane and redimensioning the sketch for the hole or cutout.

Project to Sketch is a great tool but it only works for copying sketches to offset planes, not perpendicular or angled planes. For example, if you project a sketch from the YZ plane to a plane at an angle or perpendicular to that plane, the resulting sketch will be skewed because the projection is Normal the the plane you are projecting to. In this case a circle projected to an angled plane will become an ellipse.

 

[JST]

Not only will it be an ellipse, but it may not even be where you want it to be, because of the projection normal to the destination plane. So you may lose most of the advantages you might expect to get from a projection.

 

[idslk]

Have you tried such workflow? (here from scratch)
1) create first sketch on XY-Plane
2) sketch "something"
3) extrude boss (only for visibility)
4) create new plane with Plane, axis, angle: XY-Plane, X-Axis, 0°
5') create new sketch on the new plane
6) project the "something" from the first sketch to the new sketch without association
7) extrude boss
8) Edit the new plane and change angle

 

[HaroldL]

LIke I said:

When you are adding holes or cutouts then a properly set up sketch plane will allow you to move them from one surface to an adjacent or other surface by changing the orientation angle or offset of the plane and redimensioning the sketch for the hole or cutout.

Just not the step-by-step.