Forum Index

 
 FAQFAQ   SearchSearch   MemberlistMemberlist   UsergroupsUsergroups   RegisterRegister 
 ProfileProfile   Log in to check your private messagesLog in to check your private messages   Log inLog in 

Donek Drag knife best practices

 
Post new topic   Reply to topic     Forum Index -> Equipment and Tools (e.g., ski press, core profiler, etc)
View previous topic :: View next topic  
Author Message
vinman



Joined: 09 Nov 2007
Posts: 1317
Location: The tin foil isle

PostPosted: Sun Dec 16, 2018 5:52 pm    Post subject: Donek Drag knife best practices Reply with quote

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
Back to top
View user's profile Send private message Visit poster's website
vinman



Joined: 09 Nov 2007
Posts: 1317
Location: The tin foil isle

PostPosted: Mon Dec 17, 2018 2:17 pm    Post subject: Reply with quote

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
Back to top
View user's profile Send private message Visit poster's website
chrismp



Joined: 13 Feb 2009
Posts: 1267
Location: Vienna, Austria

PostPosted: Tue Dec 18, 2018 1:25 am    Post subject: Reply with quote

Sweet, that's great news!
Back to top
View user's profile Send private message
MontuckyMadman



Joined: 20 Jun 2008
Posts: 2366

PostPosted: Tue Dec 18, 2018 8:43 am    Post subject: Reply with quote

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.
Back to top
View user's profile Send private message
vinman



Joined: 09 Nov 2007
Posts: 1317
Location: The tin foil isle

PostPosted: Tue Dec 18, 2018 9:32 am    Post subject: Reply with quote

^^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
Back to top
View user's profile Send private message Visit poster's website
mammuth



Joined: 28 Oct 2014
Posts: 306
Location: somewhere in the alps

PostPosted: Tue Dec 18, 2018 10:46 am    Post subject: Reply with quote

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.3705/videos/10100762307576850/
_________________
Tom
Back to top
View user's profile Send private message
MontuckyMadman



Joined: 20 Jun 2008
Posts: 2366

PostPosted: Wed Dec 19, 2018 9:10 am    Post subject: Reply with quote

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.
Back to top
View user's profile Send private message
vinman



Joined: 09 Nov 2007
Posts: 1317
Location: The tin foil isle

PostPosted: Wed Dec 19, 2018 12:32 pm    Post subject: Reply with quote

MM what software are you using?
_________________
Fighting gravity on a daily basis
www.Whiteroomcustomskis.com
Back to top
View user's profile Send private message Visit poster's website
skimann20



Joined: 27 Feb 2008
Posts: 338
Location: Taxachusets

PostPosted: Fri Dec 21, 2018 9:55 am    Post subject: Reply with quote

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.
Back to top
View user's profile Send private message
vinman



Joined: 09 Nov 2007
Posts: 1317
Location: The tin foil isle

PostPosted: Tue Jan 08, 2019 5:29 pm    Post subject: Reply with quote

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-360-computer-aided/adding-corner-actions-to-drag-knife-tool-paths-with-the-donek/td-p/8412208?attachment-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
Back to top
View user's profile Send private message Visit poster's website
Display posts from previous:   
Post new topic   Reply to topic     Forum Index -> Equipment and Tools (e.g., ski press, core profiler, etc) All times are GMT - 8 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum


Powered by phpBB © 2001, 2005 phpBB Group