Sketch driven hole pattern to a logo geometry line
Hi,
I have this S logo I need to "cut" using a punching machine. I want to punch the geometry line with 5mm holes (as in the phone booth image) that are 7mm away from each other. I watched multiple tutorials but no luck.. Can you help me with this one?
Another question. If I wanted to fill the whole area that the logo covers with the same holes - would that be possible?
And please, give me step by step directions - not the finished file :)
2 Answers
No problem.
Step 1. open a new sketch on the large surface of the part, select all the edges of the "S" (right click 'select tangency' is the easiest way) and create a 'fit spline' feature. This creates a single curve out of all the bits and pieces of the "S" . Close the sketch.
Step 2. 'delete face' on the surfaces making the "S" hole to eliminate it. Or create an extrude feature to fill the "S", somehow you want just the blank plate after this step. You could also go into the original boss feature and make the "S" geometry all 'construction lines' and then you don't need this step. You could even do the 'fit spline' in this sketch and eliminate step 1.
Step 3. Create the 5mm diameter cut wherever you like along the perimeter of the "S" sketch from step 1.
Step 4. Using the cut from step 3, create a 'curve driven pattern' feature. Set the spacing to 7mm, and increase the pattern count until the perimeter of the "S" is full. It should look about like the attached image.
Note, the distance around perimeter of the "S" will need to be just right for the last cut in the pattern to be 7mm from the first. In the model you provided, 29 fit the best, but the last one was a little too close to the first.
2nd question
Also easy, in Step 3 above, place the circle somewhere inside the "S" boundary and use a 'fill pattern' instead. Set the pattern layout and spacing options that you like, and that should do it.
In general, it seems like the model is too small for the stated hole size and spacing, but once that's nailed down these methods still apply.
Hi!
Thank you for the detailed directions. Unfortunately I am self learned with Solidworks and I've only done some basic sheet metal products, so after step 1 I failed / didn't understand what you mean. Also I forgot to scale the model to x10, so thats why the 5mm holes were a bit too big :)
I can select the direction to be the S but, it wont let me select the hole in the curve driven pattern to be Feature or Faces.
