- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
how to add a thread insert as new tool in turn 16el ag60
hi trying to add this insert 16el ag60 posithread in turn but the numbers do not match any one no how to do it thanks steve
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
hi yes tried that how do you do the tolerance ? and the cross section ?
i can cut the thread but it doesn't seem the wright depth please advise thanks steve
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
You'd have to do some digging on that. I'm not a lathe guy, so a fair amount of insert information is basically Greek to me....
http://www.iscar.com/eCatalog/MoreInfo.aspx?mapp=TH&fnum=113&app=0&item=5902119
I did find the solid model of the insert, if you want to try to glean any information off of that. I've attached the file
Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
What do you mean the numbers do not match?
Being a 16EL insert you need to pick the ISO Triangular Full Profile insert shape and define the rest.
As you're using an AG60 insert it comes to a "sharp" (R.003") corner. This dimension is usually given to you as "L" - Cutting Edge Length (Which on a 16 size AG60 is 0.650")
Your problem may be that you're trying to cut a Metric, or UN thread with an AG60 insert. This can work but the cam system will rely on you knowing what the difference in height from the .003" rad to the radii the thread you're cutting is by setting your thread depth correctly. Or you can just do what I do and use the book value for thread depth and use your machine offsets to bring it down to size.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
And in aluminium it seems to brake all the threads it seems like it’s cutting two threads not on please any help would be awesome thanks Steve
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Make up a model with a toolpath set up how you think it should be done with the tool in this post setup again how you think it should be.
This will give what may be wrong with the tool or the toolpath or even the model then you can be corrected or if it is a bug the cam guys have some data to use. What is in the link Seth posted is all the tool info you could ever need.
Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz
Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
hi tried making new tool, still the same it wont let me set the tool radius, don't no what the tolerance of the tool is? ,and the cross section don't no which one to choose on the fusion page can not choose if its single start ,double start,or treble start how do you get in touch with auto desk about this thanks steve unless you no any of these questions or do they mater these bits
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
You can get hold of one of the most excellent CAM staff members by doing this @jeff.pek can you please help with this.
Win10 pro | 16 GB ram | 4 GB graphics Quadro K2200 | Intel(R) 8Xeon(R) CPU E5-1620 v3 @ 3.50GHz 3.50 GHz
Daniel Lyall
The Big Boss
Mach3 User
My Websight, Daniels Wheelchair Customisations.
Facebook | Twitter | LinkedIn
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Can you attach your sample file here so we can take a look at it? Also maybe the NC code that you are expecting to see so we can trouble shoot it.
Akash Kamoolkar

Akash Kamoolkar
Software Development Manager
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
click on "browse files to attach", look for your file then click on open.
Akash Kamoolkar

Akash Kamoolkar
Software Development Manager
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
There's many issues here at a quick glance:
- An M10x1.5 thread should have a major diameter of 9.735-9.969 mm - You've drawn it right at 10 mm.
- Your OAL of the insert needs to be 16.51 mm, also the pitch needs to be 1.5 mm in the insert definition.
- Your thread depth in the cycle is set to 0.92 mm, the thread height of an M10x1.5 thread is 0.812.
- M10x1.5 thread should be made in 4 cuts, 15 is a waste of time.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
On the threading insert page you have to put in 1.5 not 3 as the insert is
Then you have to put in 16 .5 for length as it says 16 mm on there web site for that insert
So if I was doing a m10*1 I would have to go to my insert page and change the pitch to 1 and get the major dia and miner dia devide by 2 thanks for all your help Steve
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Yes, you model the work piece to the proper dimensions so the tool path knows where to start.
Yes
16ELAG60 inserts have a 16.5MM "L" value.
M10x1.0 would have a 0.541 Thread height. (Because you're using a sharp tip insert)
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Ok thanks for that I will try it tomorrow and let you no
Just one more thing you might no I have a 8 position tool changer 4 inserts 4 holes
Say on hole no 4 (8) position I won't 5 different size drills to go in no 8 position at different off sets how would you do it so Mach 3 knows all the drill of sets
Thanks again Steve
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
I wouldn't worry about the tolerance and cross section, they don't effect the toolpath.
Let me clarify what you're asking.
You have an 8 position tool changer
You want to create a tool library of your different drills
You want all the drills in your tool library to be Position 8, but call a different tool offset.
If my understanding is correct just create the drill, and in the "Post Processor" tab of the tool creation pop-up Where it says "Number:" Enter 8, and for Length offset Enter "X" Where X=whatever offset number you want it to be.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Hi just looked at my chart it seems to be different to yours is there a standard chart I can get I will send a photo of mine let you have a look in the link thanks steve
Fusion