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I got it to work here:
I used the hole feature tool to create the threaded blind hole on the white part. Then, in the bolted conn generator, I made sure to choose the "blind connection type" (boxed in the image above). For the placement option, I chose "By hole". Then I just picked a bolt out of the content center, and it chose a bolt that didn't go thru the part. I'm not sure how it decides what length to choose, but it seems to have worked for me.
Are you using the hole feature tool to create your blind hole? Are you selecting the blind hole type from the generator? Are you creating your hole at the assembly level or the part level?
Edit: I attached the example that I created, which you can see in the image above. Files are 2012.
Sorry, Trent. I let this one slip, so thank you for the reminder!
Each of the following steps were used to create the bolted connection in the assembly posted in message #4 above. You can open that assembly and follow along to see exactly what I did.
Step 1: Created thru hole for 1/4" bolt in Angle1.ipt. Used hole tool with Linear placement option.
Step 2: Created tapped blind hole in Plate1.ipt. Used hole tool with Linear placement option.
Step 3: Created BoltTest1.iam assembly file, placed one occurrence each of Angle1.ip and Plate1.ipt. Constrained the two parts together using an insert constraint between the two holes.
Step 4: Started the Bolted Connection Generator.
Step 5: Selected the "Blind connection type" option.
Step 6: Set the placement option as "By hole". This option uses an existing feature that was created with the hole tool at the part level. More on this later.
Step 7: Chose a start plane. I picked the top surface of the Angle1 part. This is the surface where the head of the bolt will rest.
Step 8: Chose an existing hole feature. For this, I chose the tapped blind hole in Plate1.
Step 9: Chose the blind start plane. This is the plane where the blind hole feature starts. I'm not sure why it's necessary to pick this...I would think that this information already exists in the hole feature that was picked. Maybe it's more for the placement types other than "by hole". Anyway...
Step 10: I didn't have to choose the thread type and diameter since the default happens to be the type and size that I created.
Step 11: Click on the spot that says "Click to add a fastener". This opens the list of bolts from the content center. I picked the hexagon socket head screw. It inserts it at the correct diameter, with a 5/8" length. More on this later. Clicked OK and the connection was created.
Now, I noticed several things as I wrote up this post. First, I noticed that after I created the bolted connection, in Plate1.ipt there is a new hole feature with a slightly different icon in the browser (has a little padlock). Apparently, it is not necessary to create the blind hole in the part before you use the generator. It will create the tapped blind hole for you. So, in step 8, instead of choosing the existing blind hole, you would choose the existing clearance hole in the angle. This serves to locate the bolted connection.
Second, the length of bolt (which is where you are encountering issues) is trickier than I thought. I think it was coincidence that it chose a bolt length for me that didn't go through my part. I thought it would use the length of my blind hole to determine the length of the bolt, but now I don't know exactly how it works... There is an obscure option to set the length of the bolt after you have selected a fastener. You have to hold the Alt key and click on the ... button next to the bolt (see the image below).
This opens a box where you can modify the length of the bolt. It comes in with a default length, but I haven't been able to figure out what determines the default (just a unintelligent preset, or based on diameter, or ?). Once you set the length of the bolt, the depth of the blind hole and tap will adjust accordingly. Also, you can adjust the length of the bolt by dragging one of the red arrows in the graphics window (see below).
I'm still learning new things about this tool as I go, but hopefully this was helpful to you.
I couldn't open your part, but I mocked up an example of a circular part, similar to what I see in the first images you posted.
You can't use the linear hole placement on a circular part like yours. Instead, you can create a 2D sketch that locates the hole on a bolt circle with radius 250mm. You place a center point where you want the hole to be, dimension it appropriately, then when you use the hole tool, choose the placement option "From Sketch". It will automatically detect any center points and create holes there. See Sketch2 and Hole1 in the Spool1.ipt part.
I recommend using sketches to place your holes, even if it's possible to use the linear placement instead. This way, you can use projected geometry from your part origin, instead of feature edges (this results in a more robust model).
It shouldn't matter if you are using a metric or imperial fastener & threads. See the attached assembly where I created a blind hole connection 30mm deep.
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