We make a lot treat holes with flowdrill.
Now we just draw a M6 and add a prefix "flowdrill".
How do you do this?
I use a Dimension prefix:
That works, but I would like to see the hole like it is in reality. So I could choose in the part environment to draw a real flowdrilled hole and the draft sees this. So I could just use smart dimension the hole.
This is a flowdrilled hole:
Can this be added in the hole spreadsheet?
I'll look at that, thanks.
The problem is we mostly use this on tubes. So in the part environment.
Would a feature library entry work for this? In sheet metal you could createa dimple and add a hole. In part you could revovle a protrusion, and add a hole.
You can add a feature to your feature library that is a combination of the dimple and the hole and re-use it.
Here's the trick to get the hole callout to say "Flowdrill M6". Start by inserting a hole. Open the Hole Options dialog. Pick the standard you want to use and then click on the button to the right of the "Standard" dropdown and bring up the Excel hole table for your standard. Find the "threaded" sheet and and you will see a column for Thread Family and a column for Size. If you have more than one thread with the same nominal diameter each one has to have its own thread family. Scroll down to, say, M6. Insert a blank line and copy the M6 line into it. Change the family in the new line to Flowdrill and change the Size to "Flowdrill M6" or whatever you want the callout to read. Close the spreadsheet and then close the hole dialog. Start the hole insertion process again, open the Hole Options dialog, select your standard and click on the size dropdown button. You should see the new size entry in the list. Pick it and insert the hole. Now a callout that includes "Thread Size" (%TS) will show the new name. For a bonus in sync, if you select the hole the label that pops up will also be the new thread name.