Pattern with fixed spacing but variable members extended till reference

Question

Basically I am making grooves for a tiny coil of diameter like 0,5mm on a small cylinder body. I have made my 'groove', and revolved it around the axis of the cylinder and then patterned it using fixed spacing (pitch).

But I have to manually adjust the length of the cylinder body sketch to make sure it doesn't get interrupted.
Let me break it down to two objectives.

I want the coil groove to be patterned automatically till a fixed reference edge/plane. The pattern cannot be interrupted midway unless it falls with 0.0Xmm of the seed pattern or 'whole'. (In other words, the last pattern cannot be broken or broken by a specified dimension 0,0Xmm. If it is broken then the wire diameter will not fit and that space is wasted.
If this cannot be fulfilled, then the length of the cylinder is automatically reduced or increased to make that happen for the last pattern to be intersected by the given length 0.0xmm or be 'whole'/'undisturbed'.

I hope it is clear now. What is the best way to go about this? Table? The first objective if fulfilled, I can do the second point manually but it would be great if there is a way to do both.

Area fill pattern? But there is no area per se because my groove sketch revolves around the cylinder 360 degrees.

I don't see a way for the total 'whole' members to be determined automatically with fixed spacing because I have to define total number of members manually.

I am on CREO 10,0.7.0

pausob · Accepted Answer

PTC_ACTUAL_PAT_MEMBERS is a feature level parameter that belongs to a specific pattern. To insert it into other relations use the [] button in the relations editor, and then look for it by pointing out the pattern feature:

kdirth · Answer

You can control it through relations. Create measurement before groove, create pattern, then create relations.

YY = (DISTANCE:FID_MEASURE_DISTANCE_1-d5-d4/2)/D14
Y = CEIL(YY)
P15 = Y

Where DISTANCE:FID_MEASURE_DISTANCE_1 is a saved measurement of the cylinder (you could also use the length value of the extrusion), d5 is the offset to first groove, d4 is width of groove d14 is pattern spacing an P15 is number of instances. A manual regeneration is required to update it when a change is made.

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