HI,
I am new to lathe programming.
Have a new CNC lathe.
Trying to build up my library with the exact tools I have for the lathe.
I can't seem to create the internal threading tool and have it represent the actual tool.
See images for better visual explanation.
And second issue may be due to the tool creation issue but when I run verification the threads have really huge flats on the minor diameter.
It looks like the tool is meant to be a full form, are you actually using partial form tips?
Here's what I see with a modeled thread and a 1mm pitch tip created in Fusion's tool library. Seems to match pretty close. The hole is 11.035 mm measured from the modeled thread (Mid limit for the minor diameter, M12x1). Depth of thread in this simulation is 0.56mm, not sure if that's correct for a full form tip but is what fits the modeled thread. Fusion's modeled threads are quite good and created on midlimits.
Don't cut threads that often but the last time I found a bug if you used a cycle in the thread operation. I found the depth was set to the total depth from the first pass so too deep. Don't know if they've fixed this in the posts.
The problem I had was when you check use cycle the depth was added to the first cut not from the minor diameter. This was not a problem if you create multiple passes using a simple thread cycle on the machine.
@akash.kamoolkar Just noticed the message in the use cycle for the thread cycle looks wrong!
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Another problem with the simulation is there's no relief angle on the tip so for internal threads it remove more material than it should.
The point doesn't look too bad but the flat at the minor diameter is removing material from the simulation because it has no relief angle.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@HughesTooling Is correct here. The threading tool represented is a full form insert and not a single point tool so this is expected.
Christopher CooperSo what do users do when they are using a regular single point insert?
With it the way it is right now, when doing an internal thread, it verify's to the user that there is something wrong with the minor diameter when they are looking at the threads because it has huge flats on the tops of the threads.
I was doing a 1" X 8 Thread. (pretty deep threads on that size.)
I think it develops bad habits to just ignore the verify and hope for the best...
I have been hearing that the Lathe portion of Fusion is supposed to be getting a big update but I have not seen or heard about what the new updates are? or when we can expect it?
@akash.kamoolkar Just noticed the width is showing on the wrong view of the tip.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@JonSchaeffer As I said above, part of the problem with the large flat on the minor diameter is cause because there's no relief on that area of the tip so it's rubbing at the bottom. Just as a test I set the custom thickness to 0.1mm and now it looks better. Probably still not going to look correct with a partial thread form tip though.
Picture from above with a thicker tip and material rubbed away. The actual V part seems to be correct and not rubbing!
Same part but a 0.1mm thick tip.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@JonSchaeffer If you use a single point tool to produce the internal thread don't you then need to clip the top of the minor diameter to get it to pass on the thread gauge anyway?
To summarise what's going on as I understand it, the tool that is defined produces a correct screw thread in terms of pitch and angle. The full form insert profile shows the toolpath clipping the top of the thread and for a user with a single point thread it does not represent it correctly but that material needs to be removed to achieve a correct thread form.
Christopher CooperSince you are using a single-point type inserts, I suppose that it's capable of a range of thread sizes, yes? Have you defined it to it's largest possible size?
@JonSchaeffer I think there is an existing ticket for the radii as it has been requested before. I will ask that this thread is attached so the discussion is not lost and then the relevant people can reach out if required.
Thanks for the feedback everyone!
Christopher Cooper
@christopher.cooperVHK2N wrote:
To summarise what's going on as I understand it, the tool that is defined produces a correct screw thread in terms of pitch and angle. The full form insert profile shows the toolpath clipping the top of the thread and for a user with a single point thread it does not represent it correctly but that material needs to be removed to achieve a correct thread form.
Trouble is it doesn't work for internal threads. If I set the tip to 3mm thick this is what the simulation shows after it runs!
As opposed to this if I set it to 0.1mm thick.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@HughesTooling Thanks for spotting this Mark, I have notified the tool library team.
Regards,
Hi All,
Just came across this disussion as I was having a frustrating time trying to get Fusion to allow me to program a turned, internal, 3 start thread based on an M5 x 0.8 base thread. As you can imagine the room to maneuvre is very tight. I am trying to use a Ceratizit single point ground tool (which is in itself the insert). I only have the option for rectagular or triangular inserts. I tried every which way, going box by box to see if I could manipulate the tip and holder to do the job. Eventually I got to the point where I was able to cut the thread in simulation, but it did wierd things to the holder. It showed the holder in the simulation coming in from the chuck side (ie up the spindle bore) but the tip carried out the operation correctly. See first image below. The tip is machining from right to left, but the holder is shown coming in from the left. This is despite being shown in the correct orientation in the Tool Library Preview. I happened upon a work around by random chance, by manipuating every parameter I could find (some also seemed to disappear as the "make shaft round" option has gone even though its shown in the simulation). I programmed the rectangular tool tip to have a width of 17mm. See second image set below. This corrected the simulation image. I have no idea if I am doing something wrong. Fusion 360 turning seems fine for simple profiles, but where tool geometry is critical to avoid collisions (especially internally), the long awaited custom tool definition is sorely lacking. It is such a pity, as the milling side of things is so intuitive. I use it mostly as a teaching tool for our undergraduate engineering students. I have avoided anything but simple parts for the turning side of things, because I find it very restrictive, and recommend other solutions for turning to our students. Hope this work around helps some poor soul out there. I am going to try and investigate this more and see if making random changes to other insert geometries expands the possibilities somewhat, but some input from an experienced Fusion turner would be great.... All the best Pat
