try to use the unfold and fold command
those will help you to make the bends flat (during the design process)
and you can locate the holes with greater precision.
Hope this helps
The shape is either an ellipse or a tear drop, difficult to pinpoint exact center. The only way would be to save the cutout pc and find the center of mass of the cut out. When you draw your circle to cut through the tank wall, draw a double circle or two rings, then when you cut it will ask you to keep or delete bodies, if you select keep it should keep the cut body within the tank wall, then see if you can select View/Show Center of Mass...
Being for a furnace, do the holes need to be round in the rolled state?
If so, then they'll need to be fabricated this way so they're circular (and elliptical & conical (in one axis) in the flat state).
If you fabricate your holes in the flat state, then the holes in the final state will be elliptical and conical.
Assuming some gas flows through these holes, will it make a functional/operational difference in your design it one method is chosen over the other?
If so, I think this should drive your design workflow.
Lastly, for cylindrical sheet metal, I usually start with a Thin Revolve (just a line of the required height, located from a centerline by the required radius).
Make sure your thin direction going is the right (thickness inboard of your line or outboard of it).
Then I do an Insert Bends with the bend radius equal to the revolve radius. You can't revolve 360°. There must be a gap when doing this method. Try 359.5°.
Remember: For unfold (& for other such commands asking for a "face"), you must select just the line used to create the thin revolve.
You can then add your holes in the round state with circular and linear patterns or just linear pattern in the flat state (after you unfold).
I'm glad you made me think of this Lingesh.. I have often wondered about that. There does not seem to be a way to do this automatically and yes it would be nice to have the centers marked automatically. I found that if I created reference points in the part flat pattern (center of faces for each hole), then began a sketch on the surface, then selected the reference points (I did it in the tree), then converted I would end up with sketch points coincident with the ref points. Then in the drawing expand the drawing view and select the sketch and "show". Now I can measure to the points. I'm going to have to play with John's method. That does sound interesting. I randomly placed my holes in a rolled cylinder using the hole wizard.
I'm thinking that you probably want to center punch your hole centers in the flat, roll, then drill clean holes to fit your fittings.
Edit:.. I wanted to add that I could not dimension to the reference points in the drawing. That is why I needed to convert to sketch points.
Thanks for the input...This one step has single handedly reduced 50% of effort for my project...