Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Drilling op goes to origin after every hole

34 REPLIES 34
SOLVED
Reply
Message 1 of 35
WillL84
801 Views, 34 Replies

Drilling op goes to origin after every hole

Hi guys, I'm using a 2-axis TRAK K3 mill and I'm using the ProtoTRAK Conversational post. My milling ops all work great now that I've gotten all my setting configured however my drilling ops always make the tool go to the origin after every hole.

 

You can see in my CAM window it should go hole by hole:

Untitled.png

But you can see from the picture I took of the toolpath on the control it drills a hole, goes back to home, goes to the next hole, rinse and repeat:

20230404_140456.jpg

Any ideas?

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Tags (1)
34 REPLIES 34
Message 2 of 35
WillL84
in reply to: WillL84

Ok so it's gotta be something with how the control configures the file when it's opened. If I check the gcode file after it's post processed there's no return to 0,0 commands in there at all

 

gcode.png

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 3 of 35
johnptc314159
in reply to: WillL84

in the haas post and machine there is an option to return home on every index.  i see in your g code T2 is on every z line.  could the be removed ??  not sure if its your problem or not, but i just threw it out there if it helps 🙂  also why the D0  on each line ??   once the T2 is loaded the offset should not change..........   i am working above my pay grade but maybe it will help !!

Message 4 of 35
WillL84
in reply to: johnptc314159

As for the D0 and T2 on each line I have no idea why that's there, that's just how the TRAK post processor works I guess.

 

Edit: for giggles I took out all of the D0 T2 and the control still does the same thing

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 5 of 35
WillL84
in reply to: WillL84

Ok so I figured out how to manually fix it. The drill op goes first line for XY position then the next line is Z for depth. It's this Z that's making it go to the origin for some reason. For giggles I deleted every other line (every line with the Z depth in it) and renumbered the events and it worked normally - going to every hole in sequence.

 

So now the question is where is the problem? Is it in the post processor or is it in the control? I've emailed TRAK letting them know about this issue (and the issue of the tool diameters not showing up in the control) but haven't heard back yet.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 6 of 35
johnptc314159
in reply to: WillL84

where is the feed rate for drilling ??

Message 7 of 35
WillL84
in reply to: johnptc314159

It's only a 2 axis machine (manual Z) so there isn't any Z feed rate.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 8 of 35
WillL84
in reply to: WillL84

Ok so after emailing with TRAK they said that the Conversational post I'm using is meant for 3-axis machines so that's why it's got the Z values but didn't indicate why the machine would go back to the origin instead of just ignoring those Z values.

 

I asked what post I should be using as there isn't a 2-axis TRAK post available and he said

 

"You’d need to contact the cam manufacturer to see if they have one that is actually 2 axis, otherwise they’ll need to make one."

 

So basically it looks like it's on the Fusion team to hopefully make the TRAK conversational post into a 2-axis version. Either that or I need to manually remove all the Z lines which doesn't sound fun at all.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 9 of 35
HughesTooling
in reply to: WillL84

This post might help.  Seems like the Prototrak post already has a 2 axis option.

 

Quoted from linked post.

 


@seth.madore wrote:

There is a Prototrak conversational post. For 2 axis use, set the user variable "useZaxis" to false and you should be good to go.

https://cam.autodesk.com/hsmposts?p=prototrak_conversional


 

Mark

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.

EESignature


Message 10 of 35
WillL84
in reply to: HughesTooling

Ok I looked into that. By default the checkbox for "Use Z axis" is unchecked. I checked it and posted then unchecked it and posted again and they're both identical when it comes to having the Z values in the drilling section. There's no Z values in the contour section though but seemingly only for the start heights. There's still Z locations for the contour paths though, just not as many. Haven't spent a ton of time to see what the differences are - maybe the feed heights are taken out?

 

testnoz.pngtestusez.png

 

I tried to attach the gcode files but it says it doesn't allow attaching .mx2 files.

 

files.jpg

 

Edit - changed them from .mx2 to .txt

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 11 of 35
seth.madore
in reply to: WillL84

Are you using the generic supplied proto-trak post processor?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 12 of 35
HughesTooling
in reply to: WillL84

@WillL84 You're using a conversational post but the files you shared are G code, is that an intermediary file or does the control just give you a conversational dialog when you edit the code?

 

Can you program the machine manually? What does the code look like if done at the machine?

 

I don't have a 2 axis protack so not sure about that but I have a couple of old EZtraks. What seems odd is how do you know what Z depth to use? With the EZTraks you program your Z depths and you are prompted to set the Z to the correct depth, milling or drilling. Can you do this on a 2 axis Prototrak?

 

Mark

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.

EESignature


Message 13 of 35
seth.madore
in reply to: WillL84

But, there are in fact differences between "useZaxis" and not:

2023-04-06_09h59_24.png

2023-04-06_09h59_40.png


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 14 of 35
seth.madore
in reply to: WillL84

Like one of the comments above, I think that your machine is not converting the g-code into something ideal for your machine.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 15 of 35
WillL84
in reply to: seth.madore

Yes I'm using the standard post from Autodesk.
Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 16 of 35
WillL84
in reply to: HughesTooling

The post puts out an MX2 file which the control then loads. I don't do any gcode on the machine itself. If I were to program that by hand on the control it'd say "set Z" at every hole position and this code does do that.

It's just after I drill the hole and hit go to move to the next one it goes to the origin then says "set x" again then I hit go again and it goes to the next hole. If I take out those lines with the Z depths manually before loading the code into the SMX control it won't do that.
Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 17 of 35
WillL84
in reply to: seth.madore

Possibly but almost everything else works perfectly. The only thing that doesn't other than this is that it doesn't show tool diameters on the control screen. I've set up everything in Fusion itself to work better with this 2-axis machine like removing all vertical lead-ins. This is the only TRAK post I've found that this machine will even accept. It pulls it right in as .mx2 format.

 

If I load it at gcode it doesn't do any conversions on the control side but then there's no Z breaks, it just runs the whole code at once with no pauses for tool changes, etc.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 18 of 35
seth.madore
in reply to: WillL84

@WillL84 could you program up a part at your machine (just a handful of drilling points) and pull that program out of your machine? What does it show? Can your machine convert a program into g-code, or is it only g-code > ProtoTrak? Share that program here, please (you'll need to save it as a .txt or .nc file)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 19 of 35
WillL84
in reply to: WillL84

Ok so the control won't save a file as anything except a .PT4. if I try saving as gcode it says it can't do it. I renamed it to a .txt and attached it. It looks like some TRAK-specific code as it's not gcode.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
Message 20 of 35
HughesTooling
in reply to: WillL84

@WillL84  I have a couple of 3 axis Prototrack machines and I use the Prototrack GCD post, can you import gcd files with your control?

 

Using this post the code comes out like this. Not sure how your control will react to the Z moves but might be worth a try.

(1001.GCD)
(GENERATED BY FUSION 360 CAM *2.0.15509)
(FRIDAY, APRIL 07, 2023 133107)
(MACHINE)
(  VENDOR XYZ3500MILL)
(  MODEL 3500BEDMILL)
(  DESCRIPTION 3500PROTOTRAK MILL)
(T09  D=8.1 CR=0. TAPER=118DEG - ZMIN=-32.433 - DRILL)
N1 G90 G94 G17
N2 G21
(DRILL16 2)
N3 M09
N4 T09 M06
N5 S539 M03
N6 G54
N7 M08
N8 M334
N9 G61
N10 G00 X35. Y101.
N11 Z15.
N12 G00 Z5.
N13 G98 G82 X35. Y101. Z-32.433 R5. P3000 F65.
N14 X-35.
N15 Y-101.
N16 X35.
N17 G80
N18 Z15.
N19 M09
N20 M30
%

Mark

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.

EESignature


Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report