Drill point thread mill programming

[Anonymous]

Hello all,

I'm about to order some thread mills from the brand Johannes Boss (http://www.johs-boss.de/en/products/thread-milling-cutters/bgf/)

On the website of the supplied we can download a programming tool, and when i use that tool i can generate some G-code which is great. But i really just want to use Fusion to program my (4 axis indexed) parts.

I mention that my parts are indexed, otherwise it would be easy to just make a sub program.

But now i'd need to readjust my Z-heights because of the offset translation.

Here's the info and code generated by the JBO tool: 

Thread definition:
---------------------------------
Thread shortcut: M 10
Type: straight
Screwing direction: right
Internal / external thread: Internal thread
Thread pitch [mm]: 1,5
Thread depth / length [mm]: 24,65


Tool definition:
-----------------------------------
Tool information: BGF M 10 (x1,5) 2,5xD IK
Order number: 400110
Cutter length l1 [mm]: 26,95
Cutter-Ø [mm] d1: 7,95
No. of teeth: 2
Countersinking length ls [mm]: 28,2
Cutting direction: right hand cutting

Machining parameters:
-----------------------------
Type of machine: Milling machine
Control type: DIN
Cooling: Internal cooling
Feed rate according to: Miller center
Milling direction: Conventional milling
No. of cutting passes (radial): One
Produce deep thread (axial): No
Tool compensation: On
No. of discharge cycle: 1

Cutting data & miscellaneous:
--------------------------------------
Material group: Aluminium
Material: Aluminium  ≤ 140 N/mm²
Cutting speed [m/min]: 250
Rotation speed [1/min]: 10010
Feed per teeth [mm]: 0,11
Feed rate (milling) [mm/min]: 469
Drilling feed [mm/U]: 0,22
Feed rate (drilling) [mm/min]: 2202
Expected processing time [s]: 3,06
Processing operations: Drilling, countersinking & thread milling
Output dimension unit: [mm]

This programme has been created according to DIN 66025. The programme is used as example for programming and should be
proved in any case of assumption before operation by simulation. The company Johs. Boss GmbH & Co. KG takes no
responsibility on the correctness of the nc-code and will not take any liability for possible occurring damage on
operation equipment or staff.

NC-Code: 

N010 T1 M06
N020 G00 G90 G54 S10010 M03
N030 X0 Y0 M08
N040 Z2.000 ;(START OF DRILLING)
N050 G01 Z-1.000 F1101
N060 G01 Z-26.947 F2202
N070 G00 Z2.000 ;(END OF DRILLING)
N080 Z-26.847 ;(START OF COUNTERSINKING)
N090 G01 Z-28.200 F734
N100 G00 Z2.000 ;(END OF COUNTERSINKING)
N110 Z-24.997
N120 G91 ;(START OF THREAD MILLING)
N130 G01 G42 X0 Y3.975 F235
N140 G02 X0 Y-9.027 I0 J-4.513 Z-0.225
N150 G02 X0 Y0 I0 J5.052 Z-1.500 F469
N160 G02 X0 Y9.027 I0 J4.513 Z-0.225
N170 G01 G40 X0 Y-3.975
N180 G90 ;(END OF THREAD MILLING)
N190 G00 Z2.000
N200 M09
N210 M30

Is there a way that i can make a custom cycle in fusion? Or should i try to "connect" two drilling cycles and a thread mill cycle?
Also, i'd like to use radius compensation, regardless of the hole size i select

(input the D dia instead of the hole in my solid. Often a M10 hole will have a 8.5mm hole in the solid. Which is not what i want to mill, i want an R5 helix with radius compensation. Of course, i don't know if i can even use the same tool in fusion for these operations.

But please, have a look at the video, to really understand what i'm tryin to program. I'm doing my best to express myself in English, even though it's not my mother language.

https://www.youtube.com/watch?v=7HVtf2RviHY

[paul.clauss]

Hi @Anonymous

Thanks for posting! Unfortunately, custom form tools are not currently supported in Fusion 360, and I do not believe you will be able to use the tool you mentioned to create a custom cycle for the desired operations in Fusion 360 without a lot of sketch geometry and manual depth selections, which would be very time consuming.

I did notice there is a Fusion 360 Ideastation post requesting the capability to use custom form tools. Please give this post a vote if you'd like to see this included in Fusion!

Please let me know if you have any questions.

[Anonymous]

Hi @paul.clauss

Thank you for your reply!

I was already afraid i couldn't make it work the way i wanted to. Is there a way i can pass G-code through to the post processor? When i use the Manual-NC form i don't seem to get it output to my posted file.

This way i can perhaps code a custom macro in my machine, and call that macro from Fusion. Or, i can make a custom drilling cycle in my post and "just" use a drilling cycle to make things work.

It's clear that i've got to find some out-of-the-box solution..

Again, Thanks for your reply!

-Peter.

[LibertyMachine]

Couple of thoughts come to my mind;

You essentially have two tools wrapped into one: A drill, and a full form thread mill.

Option 1) Duplicate tool numbers. Program a drill, assign it a number. Program a full-form threadmill, assign it that same number. A small post edit may be needed to remove a possible "tool already used" error (not sure if that will even happen) The downside to this is that you would have wasted rapid moves, as you are running through the toolpaths twice

Option 2) I'd be somewhat surprised if there wasn't a post process solution for this. Programming a thread cycle yields a toolpath that rapids to the bottom of the hole. There has to be a way to change that in the post to perhaps a long hand drill cycle. I'd definetely send an email out to the resellers in your region and see what they think about it. It's free to ask! If you are in the US of A, I'd be remiss if I didn't give a plug for Silverhawk Solutions. They crafted some rather clever post edits for me when I realized I was over my head. The prices were very reasonable as well.

[chris]

Several friends (read a dozen or so) and I with machines that do not have rigid tapping capabilities recently acquired a great deal on many of these drill/threadmill combination tools and have been trying to figure out a solution to use them with fusion as well.  I was wondering if anyone had come up with anything since this was posted a few years ago?  i know the form tool issue has been addressed since as we have already modeled the tools and similarly have the code needed for the tools but aren't quite certain how to get the proper moves through just using the multipoint threadmill operation.  we got close but were lacking the small retract move after the chamfer was completed to begin threadmilling.  everything else seemed to look like it would work OK though.  wonder if maybe a dialog box could be added to the multipoint threadmill dialog maybe for that small retract move?

Thanks for any pointers or solutions in advance!

Chris

[CNC4XR7]

I would also Like to see a Cam op in Fusion 360 for a Drill point thread mill. It seems the cycles needed are already in place if there were a way to combined the two into one cycle this would be great!

[chris]

after playing with it some more it seems like when i use the modeled form tool it wants to treat it as a single tooth threadmill rather than the multitooth threadmill.  maybe if a checkbox could be added to the form tool to treat it as a multi or single type threading tool that would also be helpful.  I think these tools are really a great benefit to the guys with no ATC as but also for guys with umbrella ATC's probably for not needing to have so many different tools in the carousel taking up pockets.  and for the manual tool change guys its fewer rapid succession tool changes.  I don't see these tools going away in the near future as they really do a great job when i have run them with the supplied manual code, but it would be really nice to be able to incorporate it into regular cam programming where it would make the biggest difference for us! so if anyone has their ears on, please let us know if we can help in anyway!  like i said there are at least a dozen or so of us trying to work out a solution for this at the moment that i know of and I am sure there are more out there probably or maybe even some who have figured out a solution?  😄

Thanks in advance!

Chris

[jameswyatthopkins]

I am also interested in seeing this feature added to the Fusion 360 package, seems that it is a popular tool for modern machining and there is noting like keeping up with the times. In addition I believe it will make an even more attractive tool out of Fusion 360. I can see it helping me particularly with parts I machine having up to 6 holes that need to be threaded. I literally could do a part and pull it from my machine completed in two setups.

[jameswyatthopkins]

Paul,

   I have this same type tool in my collection of improvement tooling to become more efficient in my small shop.

I am also interested in seeing this feature added to the Fusion 360 package, seems that it is a popular tool for modern machining and there is noting like keeping up with the times. In addition I believe it will make an even more attractive tool out of Fusion 360. I can see it helping me particularly with parts I machine having up to 6 holes that need to be threaded. I literally could do a part and pull it from my machine completed in two setups.

[CNC4XR7]

The Fusion 360 Team Is always making amazing updates from suggestions just like this Drill Point thread mill CAM op.

I can definitely see the benefit to all as the multi purpose Tooling is becoming more practical to shave valuable cycle times. I can see where just a few option boxes could be added to help move this forward. Of course that sounds simple enough to me. LOL

GO TEAM FUSION!

[chris]

I know this sounds easy when presented like this and I also know that it isn't as easy on the back end, but i think that we are really only a little move away from being able to implement this type of tooling with the existing threadmilling strategy.  if i break it down the way i see it maybe it becomes easier to see a short term solution that may not be so difficult to implement in an update? 

So for the form tool, it would need to be able to be identified and given the attributes of a multipoint threading tool with a single helical cutting pass and overlap to complete the threads.  the depth would be determined by the modeled hole which would be determined by the tools depth to achieve the correct chamfer size.

so below is just a quick representation of a checkbox on the form tool page that would indicate the tool to be given those attributes so when selected it would act accordingly.

The drilling portion, there is already an option to use a high feed rate instead of a rapid rate which could be utilized for the drilling and chamfering portion of the operation as well as the small retract move after chamfering and before threading begins.  see the option listed below:

   

The Retract move is essential to accomplishing the goal as without it the chamfer portion of the tool will make a mess of things when threading starts.  if a dialog could be added with a check box for Drillpoint Threadmilling in the operation setup with a spin box for the retract height to be entered in that woiuld be great. this retract amount would be entered in right after the z move to depth (highfeed drilling move in this scenario), and right before the lead in move began for threading.  it shouldn't be a difficult add in I wouldn't imagine??  see the example below.

Surely I know this is an over simplification, but i wanted to point out what i found to be the hangups of making this work from the most basic perspective possible so that perhaps it could be made into a short term solution and from there possibly a better more refined solution down the road?  Any help or reply or input is greatly appreciated!

Chris

[Anonymous]

I would be interested in seeing this functionality added.

[chris]

Have you guys had a chance to ponder this for us to see if there could be a short term solution for this type of threading tool?  It sure would be welcomed and appreciated!

Thanks Autodesk Team!

Chris

[seth.madore]

The best (only) workaround at this point is with Form tools. It is possible to treat it like a fullform: