I am trying to implement thread mills into Creo negating the need to use a code generator from the manufacturer, so that code can be reliably posted from the manufacturing model.
- I am having troubles setting the depth of the NPT, as there seems to be no "thread length" in the parameters, or depth option. I am not completely sure, but this depth appears to be controlled by entering the number of teeth on the cutter, in the "flute" field of the tool information. This seems like a very odd way of controlling depth, is it how it is done?
- The code generated when doing an NPT thread mill is many lines of point movement rather than a few lines of canned cycle. There is no G03 movements output at all, and this makes for a very awkward and VERY long program, any workarounds?
- Placement of the thread when choosing start and end. I am having problems with the placement of the thread, I have attached screenshot to help explain.
In this demonstration, I have made a sample part that is .500 in. thick. I will try to thread a 1/8-27 NPT into it.
Here you can see my how my tool is defined, it is an Allied TM27NPTF in case anyone wants to spec it out further.
Here are my parameters
I want a normal NPT from the top of the part down, but here is the resulting tool paths that I get. This is with start and end both set to "auto"
Here I selected the top of the part for start, and left the end as "auto", it gives me the same results as when both on auto. Note that if I try to select the bottom of the part here as the start, and leave the end on "auto", it removes the tool path
Here the start is still set to the top of the part, but now the end is set to the bottom of the part, yet the tool path is at the bottom and does not complete the thread to the top of the part.
This is the same as above, only reversed. So the start is now set to the bottom of the part, and the end is set to the top of the part. Now the tool path is to far above the part.
Lastly, we have the start set to auto, and the end set to the bottom of the part. Note that if I try to select the top of the part here as the end, and leave the start on "auto", it removes the tool path.
So aside of putting both start and end to the top of the part, or the bottom of the part simultaneously, I have now exhausted all possible combinations without achieving a normal NPT tool path. I should also mention that I also tried calculating the NPT depth and creating a plane at that depth, setting the "end" to the plane I made, but it still did not make the desired tool path.
Question 1: Yes the number of teeth sets the depth it seems. I was confused by this at first also, but it seems to work.
Question 2: make sure your parameter Circ_interpolation is set to arc_only. this make far less lines of code than points_only.
Question 3: the thread milling has always started at the bottom and cut up. I don't believe you can reverse this unless you do It with a trajectory which is the way I used to cut the NPT threads udf that made a tapered helical curve with a single point threading tool and a trajectory curve.
The way we do NPT threads now is with a cosmetic thread that just sets the diameters and depths and calls it a NPT hole of what ever size needed for 1/8 1/4 and 3/8 which is what we do the most often. We don't use the hole function for the tapered NPT. Our engineering doesn't like it I guess because you basically have to create 2 holes. The straight drilled hole and the tapered thread.
here is a 1/8 27 threadmill multi pass path picture
Neal,
not sure why you are not seeing the circ_interpolation parameter?
if you are trying to spin the thread mill all the way out of the hole then you need to look at the over travel parameters. the start_overtravel makes the cutter go deeper into the hole and the end_overtravel makes the come out of the hole.
the last picture is a .600 deep thread with an end overtravel of.6 Hope this helps with what you are trying to do.
That is exactly what I am trying to do. So essentially you have to fill out the overtravel exit, or in your example you would get no travel since it is .600 deep, and overtravel is also set to .600, take away the overtravel and it would be 0.
So what I am doing now on my end, is creating a plane to control the depth, and setting the "end" to that plane, and then the "start" to the top surface. But when I try, I am unable to get the tool path to helix out to the correct height if I match it to the depth in overtravel (my example is 0.2348 deep, and 0.2348 exit overtravel), I believe that this is for some reason related to the tool "flutes" setting again, even though I have them set to the physical number of teeth on the tool. But as long as I overtravel far enough, I will be able to clear the hole. I just hope that the "flute" setting does not affect the actual helix or TPI, since it does seem to be wrong.
I really wish I could set the "circ_interpolation", I am using Creo 3, and cannot find it anywhere, not even in tools/visibility.
It should be around the highlighted areas (and I have searched for it when reordered to alphabetic)
