I want to place this 9 slots on the face1 and face2 only, not on the face3. I used Circular Pattern tool but it is not responding as required. How to fix this problem? Part file is attached.
I want to place this 9 slots on the face1 and face2 only, not on the face3. I used Circular Pattern tool but it is not responding as required. How to fix this problem? Part file is attached.
Maha,
I didn't look at your model, but you can select "Instances to Skip" and select that instance
Hope this works
I tried this before but it did not work. Let me try again.
2nd screenshot and part file have been changed to correct the error. New construction circle is created to establish the center of the circular pattern.
Your main body is not square, so a circular pattern will not work, you could mirror to one side.
Correct, it is rectangular, not square. Each of the 4 sides needs to have the same distance from the center of rotation for the pattern.
Your best bet might be to put the cutout shape once in each of the 4 sides, then select all 4 cutouts and linear pattern them down all at once.
As Tony said, the body isn't square. You could place the slots on Face 2 by mirroring using the Front Plane, but I haven't figured out a good way to get the slots onto Face 1. They might need to be a different length anyway since that side is shorter.
I think you are correct. With just some quick measurements it would seem the slots would need to be smaller or come in contact with the corner fillets and intersect the drilled holes.
Tony is correct, you are not square so circular pattern will not work.
If the space between the center cut/circle is the same from the edge of surface 0, 1, & 2 - then you could use the temporary axis of that cylinder as you centerline and make a Equal Circular pattern of (4) four spaces, then you would need to "Skip" the forth instance, that will work only "if" that space from the edges are the same.
Otherwise you could insert a derived sketch etc...
Hi Maha, I think you can do it with this screenshot
Thank you
Solution is not clear enough. I am able to add an axis after that..........
Also I could not understand the need for axis because constructed circle is already there.
You can't use circular pattern, your feature plane - Plane 1 is shifted 3mm from the centre of the hole. Moreover, face 1 one is 0.5mm closer to the centre than the other two.
This doesn't matter since he created a center axis not referencing any of these things. Circular pattern does work as shown in above examples but the cuts will be different since it's not a square part.
So, the part is still not square, but the circular pattern is OK.
I modified your part.
Check that out.
Could you tell me please what the modifications are?
Sorry, I thought that can review it from feature tree.
Instead of cut revolve I used cut extrude. I've made one sketch for all 3 sides.
After that just linear pattern.
Yep, draw the geometry you want on the top surface, offset the cut feature, then linear pattern. That's the easiest to do, and the easiest to update if the main body changes.
This is a part of an assembly component so that I could not change as I want.
For as any questions as you have been asking.....have you had any sort of training? Any background in other programs?
If you use the "Insert Derived Sketch" - you only need one sketch that is dimensioned, the other sketches just position, then when the main sketch needs to change the derived sketches follow.....
Your main body is not square, so a circular pattern will not work, you could mirror to one side.