Donek Drag knife best practices

For discussions related to designing and making ski/snowboard-building equipment, such as presses, core profilers, edge benders, etc.

Moderators: Head Monkey, kelvin, bigKam, skidesmond, chrismp

Post Reply
User avatar
vinman
Posts: 1321
Joined: Fri Nov 09, 2007 4:16 pm
Location: The tin foil isle
Contact:

Donek Drag knife best practices

Post by vinman » Sun Dec 16, 2018 5:52 pm

So I recently got a hold of a Donek D2 drag knife. It's pretty sweet but I still have some things to figure out.

I'm using Fusion 360 to set up the tool paths. F360 does not have native drag knife support so I have to use multiple steps to get the correct corner actions added to the code.

I know there are some users here that use the Donek knives so i thought I would start a new thread on this.

I found this info posted by Donek in the cnc zone forums back in 2012 and there is some good information in here.


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.



If you have any pearls to add please share!!!
Fighting gravity on a daily basis
www.Whiteroomcustomskis.com

User avatar
vinman
Posts: 1321
Joined: Fri Nov 09, 2007 4:16 pm
Location: The tin foil isle
Contact:

Post by vinman » Mon Dec 17, 2018 2:17 pm

I emailed Donek Tools. They gave 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!
Fighting gravity on a daily basis
www.Whiteroomcustomskis.com

User avatar
chrismp
Posts: 1278
Joined: Fri Feb 13, 2009 9:00 am
Location: Vienna, Austria

Post by chrismp » Tue Dec 18, 2018 1:25 am

Sweet, that's great news!

User avatar
MontuckyMadman
Posts: 2379
Joined: Fri Jun 20, 2008 9:41 pm

Post by MontuckyMadman » Tue Dec 18, 2018 8:43 am

Sean is an awesome guy and incredibly helpful.
I use his custom macro spreadsheet because i have a shopbot to impart the cornering functions.
I had to use a different offset for my d1 than what was specified.
As he says its machine specific.
Tool path direction helps allot with laying the blade down right.
Make sure your cam outputs as straight line segments or you wont get corners to work, or at least thats what I had to do.
sammer wrote: I'm still a tang on top guy.

User avatar
vinman
Posts: 1321
Joined: Fri Nov 09, 2007 4:16 pm
Location: The tin foil isle
Contact:

Post by vinman » Tue Dec 18, 2018 9:32 am

^^MM, agreed for sure on all of that!

Yes I’ll have to use the macro also. Somehow it’s dropping the code to start the machine. I have to copy and paste it from the original file into the corners file.

Probably because of this something is also off with my feed rate. Still working out some bugs and tuning my offset as you describe.

Once I get something worth sharing I’ll post it.

I’m trying to get the Fusion 360 forum folks involved as well, a bunch of thier developers are on there.
Fighting gravity on a daily basis
www.Whiteroomcustomskis.com

mammuth
Posts: 316
Joined: Tue Oct 28, 2014 3:48 am
Location: somewhere in the alps

Post by mammuth » Tue Dec 18, 2018 10:46 am

Dough posted a nice video on fb. Im surprised how fast he cuts.

Im so free to share the fb link here, hope it works:

https://www.facebook.com/doug.smith.370 ... 307576850/
Tom

User avatar
MontuckyMadman
Posts: 2379
Joined: Fri Jun 20, 2008 9:41 pm

Post by MontuckyMadman » Wed Dec 19, 2018 9:10 am

I cut at almost the exact same speed and for more complicated and smaller die cuts.
sammer wrote: I'm still a tang on top guy.

User avatar
vinman
Posts: 1321
Joined: Fri Nov 09, 2007 4:16 pm
Location: The tin foil isle
Contact:

Post by vinman » Wed Dec 19, 2018 12:32 pm

MM what software are you using?
Fighting gravity on a daily basis
www.Whiteroomcustomskis.com

User avatar
skimann20
Posts: 342
Joined: Wed Feb 27, 2008 8:28 pm
Location: Taxachusets

Post by skimann20 » Fri Dec 21, 2018 9:55 am

One thing that I found was that my sheet cam was zeroing at the top of the material and not the top of the table. So i had to zero at top of material and run my swivel height backwards (i think).

I was giving the following info, but have to confirmed: If you go to Options->machine->post processor you will find a number of options for Z zero.


What are you guys running for swivel height. I used 0.254mm and it seemed to work well for me.

User avatar
vinman
Posts: 1321
Joined: Fri Nov 09, 2007 4:16 pm
Location: The tin foil isle
Contact:

Post by vinman » Tue Jan 08, 2019 5:29 pm

OK, so after playing with the drag knife a bit and doing a couple nights of research I have written a tutorial for those that want to use the Donek Excel utility and do not have CAM software that supports drag knives

You can read about it on the Fusion 360 forum

or you can access the tutorial at the link below https://forums.autodesk.com/t5/fusion-3 ... -id=736799

There is also a guy working on a specific Fusion 360 drag knife post processor that seems promising.

I have only cut some test squares with my knife so far. I have a couple other projects going on and haven't really had time to play with it much, especially since it has been snowing in N. VT and conditions have rebounded nicely from the December warmups and rain.
Fighting gravity on a daily basis
www.Whiteroomcustomskis.com

User avatar
vinman
Posts: 1321
Joined: Fri Nov 09, 2007 4:16 pm
Location: The tin foil isle
Contact:

Re: Donek Drag knife best practices

Post by vinman » Wed Mar 20, 2019 5:58 am

I’ve been working with a gentleman from Germany on developing a Drag Knife add-on for Fusion 360 for the past couple months. It will be released in the next few days pending approval from Autodesk. As some of you know F360 does not have native dragknife support. This add on fixed that and then some.

This add on can be used with Mac/PC. It can handle all types of geometry like lines, splines, circles, curves and arcs without trouble. It can also perform multiple depth passes for fragile or thicker materials. Swivel height, blade offset and swivel angle tolerate are able to set by the user.

This will come with extensive documentation and a workflow video.

It will be priced around $10-15 USD.

I’ll update this when it is released!!
Fighting gravity on a daily basis
www.Whiteroomcustomskis.com

Post Reply