Trouble using HOLE dialog when referencing multiple holes to sketch

[albertson.chris]

I have the HOLE dialog box up and selected "placement - from sketch"  I selected four point from the sketch at is under the body and the HOLE dialog to the right of "Face/Point" says "4 selected"   I have the diameters and depth selected, I'm making a counter sink hole.

But here is the problem:  There are no "objects to cut" listed at the bottom.   And there is an error showing saying t"There is no target body to cut or intersect."

If I go back to "placement" and select the single hole icon and click at a random location on the body then I do get the current visible body auto selected.

The trouble is that I do not want a hole in a random location.  I want the hole(s) at a location defined by construction lines in the sketch

I took a screen cast so you can see.  

[albertson.chris]

Sorry about that, here is the screen cast

[SaeedHamza]

The screencast isn't attached ( posted at the same time 😛 )

I guess this is a bug, because I remember seeing this happening once before on the forums

@jeff_strater

What do you think?

Regards

[albertson.chris]

I think this should get you to the file http://a360.co/2Ae9x1c

If not it is easy to re-create.  

1. Sketch a rectangle
2. place two construction lines that cross inside the above
3. sketch a point at the place where the two lines cross
4. use "e" to extrude the rectangle to a thick plate
5. use "h" as done in the screencast

If this is a bug then I'd image it would be top of the list to be fixed, holes are pretty common, maybe there is a work around

[SaeedHamza]

A simple workaround would be to create sketch circles and extrude cut

[jeff_strater · Accepted solution]

the problem here is that the sketch was created on the origin plane of your model.  The Hole command, when using a sketch as input, defaults to the opposite direction from the sketch normal.  When you sketch on an origin plane, the sketch normal will point toward the middle of the origin planes:

So, the Hole command defaults to the other way, which tries to cut air:

If you click on the "Flip Direction" button, it will change the direction to cut into the model:

Hope this is clear.

Jeff

[albertson.chris]

Yes, I know I could cut holes or extrude the plate without the circles
selected by every one is either counter bored or countersunk. I'll wait
a while before I result to that.

What's really needed is a fastener library. Then you just say "An M5
countersunk screw goes here."

[etfrench]

You may have to project the points to a sketch on the opposite face in order to create countersunk and counter bored holes.

[albertson.chris]

I flipped the direction and it worked, except for the counter sinks being
on the wrong side.

But now I think I understand this. Fusion drills the holes in the
"anti-normal" direction from the reference plan. That plane is determined
by which "position:" icon you select. I had assumed the holes were
drilled into the face that is pointed to with the mouse.

One question: How to project a sketch drawn on the origin to the top of an
extruded body? Some of my more complex parts have faces at different
heights above the origin so I might have to do this multiple times on the
same body.

I think until I learn how to project a sketch I can extrude in a negative
direction so sketch plane is on top.

Thanks, again.

[etfrench]

---

@albertson.chris wrote:

One question: How to project a sketch drawn on the origin to the top of an
extruded body? Some of my more complex parts have faces at different
heights above the origin so I might have to do this multiple times on the
same body.

I think until I learn how to project a sketch I can extrude in a negative
direction so sketch plane is on top.

Thanks, again.

---

The easy way is to just create a sketch on the face, then use the Project command to copy the points to the new sketch (The new sketch must be the active sketch). 

You can also create an offset plane using measurements then create a new sketch on the plane. 

The two direction Extrude|Cut operation can also be used to create counterbores on the opposite face from the sketch.