Ramp in length

[Justin Friesen]

Hi, don't know if this is a problem for everybody but I am running in metric and ever since I have updated my control nesting to 5.48 my ramp in length is now going the length of the side it cuts first. I have been running it with 5.48 for a while now but just noticed this the other day. When it ramps in it is not doing a pre-ramp plunge and then it is ramping the entire length of the first edge it cuts. I have my ramp in length set to 75mm but it isn't doing it. If anyone has a answers for me that would be much appreciated. Thanks

[Thom Davies]

Hey I had the same prob, What you need to do is set it to 2.95mm Ramp in length. Its because its reading it in impril not metric. which is 75/25.4 = 2.95

Hope this helps

Cheers

Thom Davies

[Jeremy Schiffer]

How wonderful to know, thanks Thom! We've been having the same issue, I just haven't had a chance to troubleshoot it yet. This will also fix a related annoyance, which is if you have the machine set to slow down on the final portion of the cut (as we do), it was going the full ramp-in length (76 INCHES, apparently) at about 2400mm/m.

[Justin Friesen]

Thanks Thom. I will give it a try today. I have also been wondering about how I would fix it from slowing down for the last pass, but as Jeremy said this should fix it. Thanks again Thom.

[Neville Bastian]

Is there a new version of control that addresses this issue of the metric imperial thing?
Since the last CN was released we are getting variations in our edge just as it turns and takes a new direction. The co ordinates are correct so it must be some flexing in the cutting bit. Maybe its accelerating too fast out of the corner. Maybe my cutter is poorer quality than what Thermwood uses for testing so its not showing up? We get about 120 sheets which are 3600 by 1800 before the bit is thrown away. I am happy with its performance otherwise. For $40.00 I am pretty happy.
Is anyone else having deflections in their edges on Particle board or MDF?
Regards

Neville

[Daniel Vonderheide]

Neville,

Right now Cn version 5.48 is the latest. 5.48 does contain the issue of converting metric ramp-in value and reads it as imperial. We hope to have this resolved in the next release. If your tool is leaving chatter when it turns corners, it most likel is traveling too fast. You can correct this by slowing the feedrate down or slowing down the accelerations. If you open the settigs area of CN and then click on the button that is labeled "sheet macros", you can add an Acceleration Macro to the header. The default is a G800 which sets acceleration to 100%. A G801 will set it to 90%, a G802 will set it to 80%, and so on to G809 setting it to 10%. I would start with a G802 and see if that helps. If not, Increment upwards until you find one that works. This will affect run times though as the machine is not accelerating and decelerating as fast. I hope this helps.

[Thom Davies]

Hey Neville

I am getting the same thing! We getting variations in our edges to! we still running the same feed speeds and same cutters for ages and i think its only started since we put in CN 5.48. So maybe something is wrong with 5.48 in metric mode?

Cheers

Thom Davies

[Daniel Vonderheide]

Thom,

Email me the cnc file from one of these jobs that is causing issues. I would like to look at the code to make sure it is writing correctly. Email it to program@thermwood.com Thank you.

[Neville Bastian]

Hi Thom & Daniel,
I think its not a path issue but maybe a acceleration issue or tool issue which will be difficult to duplicate at Thermwood. Maybe Thorm could take some photo's of the part appearance and a copy of his settings.
We have found the direction it goes around the board ie clockwise anti clockwise, can give different results in quality and even size of finished board. There certainly a lot to learn about router bit types, feed rates and feed in and out.
In some ways it would be good to have a option that the final pass or release pass does 5 edges. Even better was that it moved in say a nominated size of .25mm which really means the first or more cuts are cutting oversize the nominated size. This would overcome tool flexing,seeing the feed in and feed out on edge and provide a cleaner edge if melamine faced. If this was a option it would be handy for people who are more concerned about edge quality and accuracy than meeting output levels.
So Daniel, you have no time on the imperial fix? It is a real pain to your metric users. AS one of your famous American spokesman said. I have a dream, a dream where all the world will be as one. A dream where all people will use metric and think in metric. Where all machinery is made in metric sizes for metric sized material.

Regards

Neville

[Ryan Hochgesang]

There is currently no set time of release for version 5.49, however software engineering is working on having it ready within the next week or so.


Thom,

The following information was also sent to you via email after reviewing the cnc code you provided, but I wanted to mention here as well:

The spindle RPM for the 9.45mm tool which is being used at the time that the indention is cut in your part, is only set to 14,000 RPM, which seems a little low when cutting at feed speeds of 15000mm/m (Approx. 600 IPM). You should try increasing the router speed to at least 18,000 RPM to reduce deflection that could be occuring during cut of primary part and also when cutting adjacent part. Another question that comes up in this situation would be, are you using brand new tools or do you use resharpened tooling?

[David Egnoski]

Not to hijack this thread but, why would resharpened tooling be an issue?

[Ryan Hochgesang]

It was mentioned that the same feed speeds and same cutters have been used for ages, when discussing possible deflection issues and pour cut on edges, if reground tools are in the mix, I'd be sure they are being sharpened correctly etc.... I've seen before were shops have been using reground tooling for ever, then there are cut issue all of the sudden and in fact it turns out there has been some sort of change in quality for the resharpened tooling that was causing an issue. Just throwing ideas out there to consider all possibilities.

[Neville Bastian]

I can't really talk about what Thom meant by ages but we have used the same cutter for a number of years but this is meant in the context of same brand and model not same physical cutter. In my experience it hasn't been economical to pay for the bit to be sharpened as the number of sheets I can cut drops to a quarter. I can't work this out but I have given up so throw the used cutters in a drawer as I can't get to the stage of throwing them in a bin.
When I retire I'm going to glue all those router bits together and create a bar top.Fill the top with clear resin .

Looking forward to the new CN. Give it to Thom first so he can find the bugs.
Only joking Ryan & Daniel. I am sure there will be no bugs.

Better go before I get banned.
Regards

Neville

[jason galbraith]

For what it's worth we run our 9.5mm Onsrud and cheapy bits at 22000 feed 18000 spindle and 12500 plunge for White HMR pineboard 16mm and slow the feed down to 12500 for MDF 16mm. Get around 11hours cutting life out of a bit. We were running it slower but it burnt the cutters out too fast.