Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Drilling op goes to origin after every hole

WillL84
Collaborator

Drilling op goes to origin after every hole

WillL84
Collaborator
Collaborator

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
0 Likes
Reply
Accepted solutions (1)
2,201 Views
38 Replies
Replies (38)

WillL84
Collaborator
Collaborator

Ok so I posted just the drilling op with the GCD post, file is attached. The machine loads it just fine, doesn't do any translation like it does with the .mx2 files. It runs however there are no stops at the drill locations. It just runs the entire toolpath without stopping at the drill spots.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

HughesTooling
Consultant
Consultant

Looking at the code from the earlier post using the conversational post it looks like the g codes have 100 added to them. 

 

So G100 is a rapid, G101 is a feed and G102\G103 are arcs.

 

The drilling section just seems to be using rapids and not a drilling op, I wonder if the lines with just the Z should have the XY as well. You said you tried removing all the lines with Z drilling moves, does the control stop at each point? 

 

Looking at the PT4 code there doesn't seem to be any Z heights set, how do you know the depth you need to drill? Should you be setting ZEND to a depth and ZRAPID to a clearance height? Does the control give you any prompts for depth for milling or drilling?

--------------------------
BEGREC		4
EVENT		5588
TYPE		1	POSN DRILL
OK		1
XEND		25.400000I
YEND		0.000000I
ZEND		0.000000A
ZRAPID		0.000000A
TOOL		1
RPM		0.000000
CONTINUE	2
AUXBEG		0
AUXEND		0
COMMENT		
FIXTURE		0
ENDREC		
--------------------------

 

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


0 Likes

WillL84
Collaborator
Collaborator

If I delete the Z depth lines it does stop at every hole but it makes it so it doesn't go back to the origin between each one. That extra Z depth line is seemingly making it go back to the origin for some reason.

 

As far as Z depth these machines have a glass scale on the Z axis so the program only does XY positioning. Once it's in position a little popup comes on the screen that says "SET Z" then you manually move the quill to the desired depth using the DRO going off the print. Then hit the go button and it moves to the next location.

 

Here's the screen when you get to the drilling XY position (also for milling, it'll move to the start point then have the same "SET Z" message so you set the Z depth and hit go and it'll mill):

20230407_122131.jpg

And a shot of the machine itself:

20230407_122153.jpg

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

HughesTooling
Consultant
Consultant

I have a ProtoTrak lathe and it using a similar conversion process where you import G code (.cam) and it converts it to the conversational format. I wonder if what's happening is because the lines with the Z move don't have an X or Y they are defaulting to X0.0 Y0.0 when translated to the PT4 format.

 

After the conversion can you view and edit program at the control? With my lathe after importing the .cam files you can and save the edited program as PT4.

 

My EZTraks are similar to what you have with a DRO scale on the quill but the control stops at any Z change and prompts you with the new Z height to set. Seems odd the ProtoTrak doesn't do something similar.

 

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


0 Likes

WillL84
Collaborator
Collaborator

Maybe that's it? I'm not sure honestly and I have no idea how to edit the post to not put those Z depth lines in. We al have a Trak lathe here - a 1630SX. Only a few hiccups relating to Fusion programs but it was mostly just specific settings in the tool paths. 

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

WillL84
Collaborator
Collaborator

@HughesTooling wrote:

I have a ProtoTrak lathe and it using a similar conversion process where you import G code (.cam) and it converts it to the conversational format. I wonder if what's happening is because the lines with the Z move don't have an X or Y they are defaulting to X0.0 Y0.0 when translated to the PT4 format.

 

After the conversion can you view and edit program at the control? With my lathe after importing the .cam files you can and save the edited program as PT4.


Looks like that's exactly what's happening. If I go and view the program it has the XY position then the next event has 0,0 for XY. So the post needs to be modified to not include the Z lines when the "Use Z axis" isn't checked.

 

20230407_141106.jpg

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

HughesTooling
Consultant
Consultant

@seth.madore  Would you be able to help with a post mod? I haven't done any lately so a bit rusty with modding the posts.

 

Thanks

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


0 Likes

seth.madore
Community Manager
Community Manager

So something like this would be okay?

PN1001 G20 ;
(T7  D=0.2362 CR=0. TAPER=45DEG - ZMIN=-0.0472 - CHAMFER MILL)
(RAPID MOVEMENT TEST)
N1 G100 X-1.714A Y0.7298A D0 T7 ;
N2 G100 X0.A Y-0.7298A D0 T7 ;
%

Seth Madore
Customer Advocacy Manager - Manufacturing
1 Like

seth.madore
Community Manager
Community Manager
Accepted solution

If so, here's this file that will not output Z moves in drilling


Seth Madore
Customer Advocacy Manager - Manufacturing
1 Like

WillL84
Collaborator
Collaborator

Just tried that post out and it works perfectly. Thank you!

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

WillL84
Collaborator
Collaborator

Now that that's fixed is there any chance you could get it to actually show the tool diameters in the control? They're all listed in the gcode header but in the control they all show up as "Load Tool Dia 0.000"

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

seth.madore
Community Manager
Community Manager

Would you know the trigger for getting that data to display in your machine? Meaning, is there anything you can input manually into the g-code that will change the "Dia. 0.000" to something else?


Seth Madore
Customer Advocacy Manager - Manufacturing
0 Likes

WillL84
Collaborator
Collaborator

I'll play around with it and see if I can figure something out. Right now this is what it puts into the header:

 

PN1001 G20 ;
(T1  D=0.25 CR=0. - ZMIN=-0.25 - FLAT END MILL)
(T4  D=0.332 CR=0. TAPER=135DEG - ZMIN=-0.25 - DRILL)
(T7  D=0.136 CR=0. TAPER=118DEG - ZMIN=-0.25 - DRILL)
(T10  D=0.25 CR=0. TAPER=45DEG - ZMIN=-0.04 - CHAMFER MILL)
Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

WillL84
Collaborator
Collaborator

So I can manually enter the tool diameters and types in the tool table on the control after opening the program file so I guess that's not a huge deal. It'd just save a step having them all populate automatically.

 

It does register the tool number though, just not the diameter or type.

 

Edit. I made up a simple program on the control and saved it to the USB. It seems to put the diameter on the line instead of in the header.

PN0000 G20;

G130 X+0.0000 Y+0.0000;

G131 XM0.0000 XN0.0000 YM0.0000 YN0.0000 ST=00000;

N1 G100 X+0.0000A Y+0.0000A D0.2500 S0 T01;

N2 G100 X+3.2000A Y+5.2000A D0.3750 S0 T02;

N3 G100 X+26.0000A Y+2.0000A D0.2410 S0 T03;

%

 

It also doesn't seem to save the tool type, just the diameter. I cleared the tool table and loaded the program and it loaded the diameters but not the type which isn't a huge deal.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

WillL84
Collaborator
Collaborator

Ok I figured it out. On every gcode line after the XY positions it has "D0 T& (tool number). If I put in the diameter at the D0 (change D0 to D0.250 for example) then we now have D0.250 T7 and the control populates the tool diameter.

 

So this: 

 

N1 G100 X0.75A Y-1.5002A D0 T4 ;

 

 

Becomes this:

 

N1 G100 X0.75A Y-1.5002A D0.3320 T4 ;

 

 

And that works. Also it doesn't need to be on every line. Just having the diameter in the very first N line for the op will populate the tool table.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

kniesmachine
Observer
Observer

Will,

 

I have been following your posts on here as I have the same questions you have had with Fusion 360.  I tried the new post with a drilling operation and it did not change it from going back to the origin/first hole everytime.  What am I missing?

0 Likes

WillL84
Collaborator
Collaborator

I'm not sure honestly, I've been using that "No Z" post since it was posted and it's worked great

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes

kniesmachine
Observer
Observer

Thanks for the reply. 

 

Also, have you figured anything else out on the tool diameter besides manually entering? Have you made any adjustments to that post since 2023 to make it better?

0 Likes

WillL84
Collaborator
Collaborator

Haven't figured anything out with that, the stuff we do doesn't have a ton of tool changes so it's easy enough to keep track of manually.

Windows 11 Pro 64-bit
Inventor 2024 Pro (PDMC)
TITAN Computers C161
i7-11700K/32GB RAM/Quadro RTX A4000
0 Likes