Adding corner actions to drag knife tool paths with The Donek excel macro

[WhiteRoomSkis]

I'm wording if anyone has played with the Donek excel macro to add corner actions. To their drag knife tool paths? https://www.donektools.com/free-cnc-router-software/links-2/

it it seems like this could be done but honestly it above my computer/file manipulation/tech geek skil level right now.

is this possible in F360? I'd like to buy this knife if only I knew how to add corner actions to the  g-code that F360 produces......

any help is appreciated! Thank you!

[WhiteRoomSkis]

So I have been playing with this a bit and here is what I have found out.

I have been able to generate a trace tool path within F360 and edit it with the Donek excel macro to add the corner actions. Then I can take that file and run it through NC viewer where I can see, in the code, the (G 01) Z moves and (G 03) arcs that are generated to lift and swivel the cutter to the next vector to be cut.  If I zoom in I can also see the actual tool path which looks correct. This edited file is then able to be loaded into Mach 3 as usual.

What I have not done yet is test this on the machine since I don't have my knife yet. But for what I can see in the code and in the sim this should work.....I hope.

Somethings to be sure you do when learning this process

1. watch the Donek Video
2. You must have Microsoft Excel on your windows based computer, the Donek macro won't work for Macs
   • I think it should work to generate Code in F360 on a mac and take it to your PC to run the macro before loading it into Mach3.  (haven't fully tested this yet but it seems to work out ok with the NC viewer simulation.)
3. Be sure you set your Z to the table surface on your model or the code will not generate correctly.
4. You must use the trace tool path for this to work correctly
5. It probably doesn't require a special tool since the center of the tool is following the center of the vector in the trace toolpath. I just made a very thin flat end mill of .2mm but you could probably use any end mill you already have loaded in your library.

If any other drag knife users have good tips to add here please do so. I'm hoping this thread will help others on here who are looking for drag knife support  and want to use corner actions.

I'm hoping some one here will comment on blade alignment for the initial cut. I'm guessing the blade should be very close to aligned to the initial vector to be cut...

I'll update this as I learn more about this toolpath and using my drag knife.

[WhiteRoomSkis]

info posted by Donek in the cnc zone forums 

The best practice is as follows:

surface or fly cut your table to ensure it is totally flat and true to your machine (most important step)

zero your cutter to the table surface, not the top of your material.

make test cuts in your material, lower or raise your blade until the knife is just barely cutting through the material set this position as your z-zero

Vectric Gadget settings:

be sure you set the z zero to the bottom surface of your material and be sure to enter an accurate value for thickness

never rely on the manufacturers stated value, measure the material with a caliper or micrometer.

In the drag knife gadget:
set cut depth to the material thickness (the same you enter previously)
swivel depth should be between 0.001in and 0.010in depending on the flatness of your material and how consistent it's thickness is.

passes should generally be 1 unless you are cutting particularly hard materials

blade offset varies from machine to machine and is dependent on the model you use (see below)
tolerance angle should be left a 20deg
select a tool with a feed rate in the range of 3 to 5in/sec (180 to 300 in/min, or about 6000mm/min)

Additional advice on cut order and start points

select your paths in the order you want them cut.

it is always wise to cut internal components before external components

adjust the start points of your vectors to be in the middle of a line or large curve

the vectric gadget likes to start cuts at corners, but fails to reorient the blade at the end of the part resulting in an incomplete corner

adjust the start points on all vectors such that they begin and end in the same orientation
this reduces the need to reorient the blade at the beginning of a cut and makes your tool paths begin and end on top of each other.

keep in mind that the vectric gadget will cut all closed paths in a counter clockwise direction

Advise on determining blade offset for your tool and machine.
The best starting point for a D1 or D3 tool is 0.065in
The best starting point for a D2 or D4 tool is 0.160in

depending on backlash and other factors in your machine, these values may not be accurate enough

The best way to fine tune this value is to cut test pieces. I recommend a 1.5in square.
observe the tool in action

if the tool turns too much at a corner, then the offset value is too large
if the tool does not turn far enough at a corner, then the offset value is too small

typically adjustments of 0.005in are recommended.
repeat your test cut.

[WhiteRoomSkis]

Update: 

Use 2d countour I stead of trace. This allows you to select your entry points. Trace does not allow this. You must turn off  compensation to allow the knife to follow the center of the tool path.

the Donek excel macro seems to drop the g-code block to start the tool path. I’ve had to manually add this back in by copying it from the original .tap file and pasting it into the edited file with corner actions.

if anyone has info on this please share it.

I’ve emailed Donek to see if they would be willing to collaborate on a F360 best practices tutorial that could’ve shared here and on their website. So we will see what happens with this.

[WhiteRoomSkis]

Donek Tools has replied and they are willing to assist in working on a best practice tutorial for F360 to generate proper corner actions g-code for their drag knife based off some of the info I’ve pieced together from various sources.

stay tuned!!

it would be great if someone from F360 development would possibly help out with this.....

I think a lot of users here would benefit from this collaboration.

[WhiteRoomSkis]

OK, I am working on a tutorial to take 2d contour .tap files from F360 run them thru the Donek Macro and output something with correct corner actions. I have most of the F360 2d contour setting figured out and have screen shots and explanations of the setting for the tutorial. This should be pretty helpful to anyone that uses F360 and wants to use Donek drag knives once it is complete and tested.

Now I need some help. I know very little g-code. As described in the macro instructions The Donek Macro deletes and header information including feed rate generated in F360 resulting in the Mach 3 not starting the cut file.

I need someone with more knowledge of g-code to help me figure out this part of the process. I need to know what goes into the comment Code lines and Header lines in the Donek Macro. My gut says this is where I would put the code to start the program and define the feed rate but, honestly I have no idea. I'm a ski builder not a coder. Donek is in the process of moving their facility so I'm getting only sporadic communication with them.

There has to be someone on here the has interest enough in this to help me take this on.

if you are willing to help me out please email me at vin@whiteroomcustomskis.com

[macmanpb]

I am thinking about to change my mach3 post processor.

If it works then i have it as an option in the mach3 post processor to add this swivel-moves on Fusion360 posts.

Some thoughts about that...

1. We have two facts, a previous cut and the next cut. That routes decides the angle of the swivel and the direction.
2. In the post processor we need a look ahead. I don't know if that is possible. We need some experts?!
3. If we know the previous and the next cut we can add the swivel/tip combination move in between.
4. The form fields about the material thickness and tip offset can also be added to the post processor options as well.

But this is in theory for now 😉

[WhiteRoomSkis]

I like your idea of writing a new post-processor. I have no idea how to do that though. There's a post-processor for ArtCam which is an Autodesk product, but it looks like it doesn't really do much, you still have to run the code through the macro.

Do you have any info on what needs to go in the comment code and header fields in the macro.

If I had this info I feel like I would be 90% of the way there with my tool paths. I think I could also for the most part finish the tutorial and have some folks test it to see if it seems like the info is valid enough to share.

[macmanpb]

I don't know what you exactly mean with "macro". Did you mean the donek excel file that you have?
I want to clarify that, extending the post processor is an idea and stay or falls with the look ahead ability?

@jeff.pek, @LibertyMachine:

Are any post processor experts out there they can give me an answer whether a "look ahead" is possible?

UPDATE:

In the meanwhile i don't think we need a "look ahead". It's simpler to keep the last move. Then it is possible
to look at the previous move and calculate it with the current move and insert the swivel movement in between.

Hoping to keep the last move is possible?!

[WhiteRoomSkis]

Yes, the Donek worksheet is essentially a macro that looks for corners in the tool path and adds code for swivel moves .

[WhiteRoomSkis]

Still making progress on the tutorial.

Found this tidbit in the Donek Tools forum posted in 2015

"There is an updated version of the g-code swivel program on the web site. In all of the versions, however, you simply need to enter a metric value for your swivel height and offset to get it to function. If, this is not working, please e-mail me a copy of you source and output file, so I can track down the situation and correct it."

[WhiteRoomSkis]

I've attached a draft version of the tutorial I have been working on. It still needs some work in a couple areas. You'll see important points and areas that need to be tested or figured out still in orange text.

I have been successful in generating corner actions and cutting 1.4mm plastic sheet material with this code. There's quite a few steps to it but isn't all that complicated I hope my tutorial is easy enough to follow. I've included information that I have found while researching multiple user forums around the web that have all contributed to figuring this out.

The only thing that I really still need to figure out is how to control the feed rate. My guess is this needs to entered into the header field or added manually into the g-code with a text editor. If anyone knows how to do this please let me know. Right now my feed rate defaults to 254mm/min. I have no idea where this feed rate comes from as there are no F commands in the code to indicate feed rate

Please test my process and verify that this work for you. If you see anything that does not work or needs to be edited please let me know. I'll update this as I get the rest figured out.

Happy cutting!!

[WhiteRoomSkis]

OK have figured out where to add feed rate in the code. Feed rate needs to be added to the end of first line that starts with G1.

I have a finished version of my tutorial now that I have figured out feed rate. See attachment below.

[WhiteRoomSkis]

I've been playing with this some and you can copy the header information from the original file to the header fields in the excel worksheet and it will be placed in your new file

I'm still trying to figure out if Feed rate can be added here

copy and past this info from your oriingal file into the donek worksheet

[macmanpb]

I have tested a mach3 post processor if it is possible to store the previous move in a variable. And it works!
This is the base of developing a trailing knife post process feature.

I am still working on it and i hope i will finish it soon.

[WhiteRoomSkis]

Wow that's great news!!! I have been in touch with Donek Tools about my tutorial. They are pretty stoked on it and will be sharing it on their website soon after they test and verify the process.

I'm sure that would love to hear about your post processor and might be willing to host it. This not only benefits us but them as it may result in some sales for them. The more CAM platforms that are supported for them the better I think.

Once you feel you have a finished product I would love to test it out!!!

[macmanpb]

@WhiteRoomSkis After a lot of tests and smashing my brain against the wall i have a first version that seems to be ok.

I have added the options right into the post data.

Here a swivel test image.

[WhiteRoomSkis]

That is awesome!!!! 

Think its ready for wider testing?

[macmanpb]

At this time it is an early version that can handle only lines.

The next step is to handle inline arc's and curves correct.

But i think the hardest part is done. Hope that the other parts are simpler.

I keep you informed... 

[macmanpb]

Hi @Anonymous.p, @LibertyMachine

i have a question about 2d-contor and trace.
I am using the Mach3 post processor and saw that 2d contour uses arc's with G2/G3 with IJK but trace does not.

Trace uses small segments for arc's instead of IJK.
Is that behavior bound to my Mach3 post or what is the reason for that.