These questions are partly SE and partly general good practices. I'm trying to place holes and shell this part according to this drawing:
Ok, so here is the best practices question. To a novice like me, the only way I could place the initial hole was to place one hole on the bottom edge, mirror the hole with respect to the plane going through the part, and dimension 3.82. Then I was going to delete the second hole and use Along Curve Pattern to add the rest. Here is my part:
Is this way you guys would have initiated the hole pattern?
Now for the SE questions.
Is there a command to convert the outer edge of the base to a sketch, which can be used along with Offset to create my construction box for the hole placement?
Can a closed path be used as the "Curve" for pattern fill? Where would the anchor point be?
How do I "shell" the part without shelling the base? I tried Thin Wall and clicked on the bottom of th part, but it hollowed out everything including the mounting base.
Solved! Go to Solution.
The command you are looking for in sketching is called Project to Sketch and is the one directly to the right of the Offset command on the Draw area of the ribbon bar. For the pattern along curve, your anchor would be the first hole. I have no idea what purpose creating a second hole, mirroring, and then deleting one accomplishes, so I have no input there....
To shell the center without shelling the mounting flange, the wall value in the Thin Wall command must be more than the mounting flange thickness- in your case 0.079, if you have drawn it properly- or the command will thin the flange as well.
I agree on all the points.
Also I have found (verified by my VAR and coworkers) that synchronous thin walls can be problematic with later changes. Maybe some sync experts can chime in.
And I guess you should add the flange after the shell?
I guess the hole copy is to derive the symmetric dimension? Just dimension the one hole from the xyz base. Use the symmetric diameter dimension if you want to see the total distance.
Just place the single first hole approximately. Then dimension to it from the origin. Then edit the dimension and key in "3.820/2" and it will go to the right place.
Of course this is sort of an academic exercise, since 3.82 is the only dimension given. it assumes the length along that midline curve is exactly divisiable by 3.82 (which presumably it is, in this particular exercise).
With @Chally72 's help, I was able to create my offset hole pattern. With the intial hole selected, I clicked on Pattern - Along Curve - Chain and selected the new path. Now it's asking me for the anchor point. I'm assuming the anchor point is where the first hole is located, but the only locations where I can click are the points where the solid lines meet the curves.
How do I make the center of the current hole the anchor point for the pattern?
In the Home -> Draw group use the Split command to split your straight line of the curve passing through the hole at the centre point of your hole. This will then give you your pattern anchor point.
After splitting the line, then use Relate -> Connect to tie the ends of your split line to the centre of the hole so that if you then ever move the hole, the anchor point on the curve will follow the hole.
@uk_dave Thank you. Once I split the line, the pattern worked great. I wasn't able to tie the end of the line to the center of the hole. Could you explain the steps? I wasn't able to select the center of the hole to connect to the endpoints. I tried clicking "C", but it didn't select the hole's center point.
If you cannot actually pick the center of the hole, check your Sketching -> IntelliSketch settings and make sure you have Center turned on so you can pick the centre of the hole.
If the two are already coincident in space in my experience I usually have to move one away a little. In this case the line end. Then apply the relation.