I'm trying to make a concentric mate with the flag and the hole in the mailbox. When I select mates it won't let me select the hole or the sketch I used to make the hole to use for the mate.
I'm trying to make a concentric mate with the flag and the hole in the mailbox. When I select mates it won't let me select the hole or the sketch I used to make the hole to use for the mate.
Try selecting the inside surface of the hole instead of the edge.
The only mate available for that is tangent and that's not what I want.
Use the sketch point in the center or use the sketch circle itself...
Steve C
It won't let me select sketch 2 on the body part. (The sketch circle)
Why Eric? Is it just not shown? If so, turn it on.
Steve C
Because that is not a round hole, it is a cut you created using the Wrap feature.
At first I cut it using the extrude cut feature. I just tried wrap to see if it would work. I still didn't work.
Use the Hole Wizard...
It works just fine, assembling it when the circle you sketched is extruded as a cut...as long as you do not select the EDGE of that hole. Select the actual round face created by the cut and it works...
In short...stop selecting edges and start selecting faces.
The edge that is picked is on a curved surface so it is not a true circle and won't see a concentric mate.
How do I put the flag in the hole?
You may find it easier to change the model than to find a way to select something that doesn't want to be selected. Can you just delete the existing feature and add it back as a hole or circular cut?
Walter Fetsch wrote:
You may find it easier to change the model than to find a way to select something that doesn't want to be selected. Can you just delete the existing feature and add it back as a hole or circular cut?
Can you attach example illustrating your "solution"?
Make an actual, round hole...and it works.
You mean using hole wizard? It only lets me use the hole as a 3d sketch, which is really hard to work with.
Not that hard Eric...
Pretty dang easy...
Put the point on the face where the hole starts
Create a dimension from the front face of the mailbox to the point
Create a dimension from the flat bottom face of the mailbox to the point
Hole type, Simple
Hole Diameter, 1.06"
Hole Depth, Up to Next
It took 10 times longer to type up this response than it did to actually make the hole.
sad- just my opinion
YYURYYUBICURYY4US
kelef
Yeah...I know...
Making that hole should have only taken 1/50th of the time it took to create the email.
That works well for making the hole. I still can't mate it. The only mate is tangent.
For the mate, select the FACE of the HOLE.
(You selected the face of the chamfer, which will not work because it is not round/cylindrical)
And the FACE of the split round on the flag.
Using 3D sketches is only hard because you don't understand how to use the tool yet. Let me give you a couple of tips.
Try to always draw sketch lines along the X, Y, or Z axis.
Just go into the 3D Sketch in your hole wizard hole and create some lines:
See my line starts off on the Z direction on the ZX Plane:
Now once I terminate that line by left clicking I can switch directions by rotating the view (use middle mouse button to rotate view).
Now that I've got the view rotated almost perpendicular to YZ I can press Tab to get it to switch to YZ:
Before:
After:
Now I move the cursor until I get the yellow Along Y relation:
Then do the same along X and make it coincident with your point. Add dimensions to your sketch lines and you have a fully defined hole.
Doug Seibel's solution is a whole lot easier than what I posted. You should mark his response as correct. However, you may want to try going through my above answer because you need to understand the basics of 3D sketches and you should not be afraid to use them.
Every once in a while, I notice an issue in an assembly where a threaded hole becomes the equivalent of transparent....only the interior surfaces of the hole. Basically, all selection will go through it.
Either hold down SHIFT when you go to select it, or open the part and edit the threaded hole, then exit the edit command without doing anything, then go back to the assembly.
Is that your issue?
What about turning on the temporary axis of both and mate to them , then turn them off?
For the mate, select the FACE of the HOLE.
(You selected the face of the chamfer, which will not work because it is not round/cylindrical)
And the FACE of the split round on the flag.