Even though it is a 2D sketch what is the purpose of having Pierces relation.

SolidWorks Tutorial # 292: Shelf holder / (2 methods , sheet metal) - YouTube

Time 8.40-11.20

Even though it is a 2D sketch what is the purpose of having Pierces relation.

SolidWorks Tutorial # 292: Shelf holder / (2 methods , sheet metal) - YouTube

Time 8.40-11.20

The pierce is there to capture a relationship to a perpendicular line that isn't on the Sketch Plane, so you could have a horizontal sketch line or Model Edge in the front plane and when you add a hole or a line in a Sketch in the Right Plane you want to relate a sketch point to the line in the Front Plane and to do that you would need to turn the model slightly and pick the line and the sketch point and then the Pierce option comes up...

You're showing the model in "Shaded View" so I can't see behind the face shown, so my question to you - Is there anything on the other face, a line or a feature or a sketch... If not then my thought is that it shouldn't show up at all and if it does, I'm not sure what it would want to pierce..

Ok - That is what I thought I saw - you have multiple sketches - so you would be able to pick another line from one of the other sketches for a pierce relation.. If you would only have had one sketch showing, then the pierce relation would not have come up...

See J. Mather - reply

Edit your last sketch and double click on one of the Pierce relations.

Rather than add coincident between endpoints - you added coincident between line from previous sketch and endpoint in current sketch.

This leaves the line in current sketch with one degree of freedom (it can still translate along line from previous sketch).

You then added a Pierce between endpoint in current sketch and line in previous sketch - this removed the degree of freedom.

You could have done this in one relation instead of two by either-

using Coincident between endpoints (rather than to line) as your first relation

or

using Pierce between endpoint and line as your first relation (rather than as second relation).

J. Mather wrote:

This leaves the line in current sketch with one degree of freedom (it can still translate along line from previous sketch).

What is meant by

**one degree**of freedom?Any object in space initially has 6 degrees of freedom.

It can translate (move in straight line) along X, Y or Z axis and it can rotate around X, Y and Z axis.

Defining our geometry is an exercise in removing or allowing desired degrees of freedom (DOF).

If we start a 2D sketch on say, the XY plane - we have already removed one degree of freedom (cannot translate along Z axis) and two rotational degrees of freedom (the 2D sketch can only rotate around Z axis).

We add additional constraints to match Design Intent.

This same logic is then carried forward into 3D with assembly relative motion between components.

This is usually covered in the first 10 minutes of sketch instruction and in the first 10 minutes of assembly instruction.

I think it is worth noting that I didn't have some reservoir of prior knowledge that "gave" me the answer.

I opened your file and

1. Experimented with your Relations

2. Observed the results

3. Reported observations.

When you can do all of this (steps 1-3) on your own, then you are ready grasshopper.

Edit your last sketch and double click on one of the Pierce relations.

Rather than add coincident between endpoints - you added coincident between line from previous sketch and endpoint in current sketch.

This leaves the line in current sketch with one degree of freedom (it can still translate along line from previous sketch).

You then added a Pierce between endpoint in current sketch and line in previous sketch - this removed the degree of freedom.

You could have done this in one relation instead of two by either-

using Coincident between endpoints (rather than to line) as your first relation

or

using Pierce between endpoint and line as your first relation (rather than as second relation).