Hello All,

I have been setting up an MDF door with a beveled profile on the inside of the rails. I am having trouble with the square corners. The tool is a 140 deg. included angle carbide insert that comes to a point. I am using Enroute for the CAM side of things and it automatically calculates the 2 passes required to reach the depth I am going & the corner operation based on the tool geometry. However the 2 passes on the rail don't seem to line up and it's cutting too much into the corner.

My first instinct is that there is a discrepancy between the tool and the DXF supplied to me by the tool company. But they assure me that is not the case. I have back plotted the code into CAD and verified it that way and it seems the code is good. The guys at Enroute suspect the tool as well. I have made a number of programs using different geometry for the tool, different angles & flat on the bottom instead of a point. Some are better than others but so far none is perfect.

I am disinclined to think that the CNC is th problem as if it was i don't think that it would be so consistent on all corners & edges. But nonetheless Thursday I am going to take the tool to another shop and test it there as well.

I have uploaded a couple of pics. The worst looking one is using the geometry provided by the tool company. The better looking one I made some adjustments to the geometry.

I am kind of stuck in the middle here and not really sure what is causing the problem. But I can see it will be up to me to resolve it!

Any thoughts or ideas are welcome.

Thank you

View higher quality, full size image (1965 X 2620)

View higher quality, full size image (1754 X 2339)

Any time that happened to me albeit in Aspire it was the angle supplied with the tool was wrong so to dial it in I would tell Aspire it was 139degrees, 139.25 degrees, 139.5 degrees in .25 degree increments up to 141 degrees. I would draw 150mm square panels and run the program till I got it right. Then I'd scribe the correct angle on the tool for further set ups

Z height calibration is critical for V bits. Also have a look at the tip with a magnifying glass to see if there is a flat or damage. Adjust the bit profile in the software or change inserts.

Thanks for you replies.

I have managed to get a little further with this.

Firstly I took the tool to another shop and got the same result. So I assumed that the tool was the issue as suspected.

However after running more test pieces at different angles I couldn't get anything decent and the tool company were quite sure that the insert was good. So I removed and reinstalled the insert. I am now getting much better results on the rail where the 2 passes overlap.

Where I still have a problem is the corners. I have noticed quite an improvement when reducing the speed of the corner operation. So I suspect maybe there is an issue with that. Possibly the 3 axis move just requires more power. What speeds would you run this operation at? The tool is a single wing, 1" diameter, carbide insert.

Also is anyone familiar with any parameters on the CNC that may effect the motion on these 3 axis moves? The control is a Syntec 6MB.

Thanks for all the help

I have run an Amana 1.25" dia single flute 90 degree bit at 12000 and 150 in/min in Mdf. I got fair results doing mitre folds with two passes.
With the corner clean up passes are they small, incremental vectors as the tip of the bit rises up the inside corner? if so, the cnc will never reach the programmed feedrate because it will be subject to acceleration/deceleration.

Thanks Thomas.

I have found that I am able to get significantly better results by setting the speed very low, 10 IPM @ 12000 RPM! Obviously I am running the tool at a a lot faster speed initially so as not to burn it out. Then I am coming back to do the corners at the slower speed.

I understand what you are saying about the tool never reaching the programmed speed on those small moves. But nonetheless reducing the speed is making a huge difference. The CNC tech has suggested that when it's making these 3 axis moves it draws a lot of power and if the voltage is low it may not get distributed to the drives equally.

My next challenge is that in order to clean the corners automatically using Enroute I have to use a 3D Engrave strategy. This strategy doesn't allow you to set a different speed for the corner clean up so it has to travel all the way around the door at 10 IPM. I did quick calculation on a 30"x15" door and figure out would be around 7 minutes just to clean up those corners! Ideally would be able to set a speed just for 3D movement. I will contact Enroute and see if that's possible. If not am wondering if I can create a 3D Engrave strategy from open geometry. If so I can create an L-shape in each corner and then I wouldn't have to run all the way around the door at 10 IPM.

We'll see how it goes!

That's painfully slow. Can you manipulate the drawing to block out the corners as boundaries for the prismatic cut then run the rest at a faster pace?

120ipm, 16k rpm. Amana 60* insert tool

Mozaik generating the file.

I don't think it's a feed issue? 10ipm is crazy slow. I think it's a geometry issue. And like others have said, on a short line like that, It's not getting up to full travel speed.

I take the perimeter with a 1/2" down, 1/4" down, 1/8" down, the angle tool. Take out the pockets. Cut out the door.

View higher quality, full size image (4032 X 1908)

Hi Karl,

I am fairly confident that I have eliminated any issues with the geometry. I am running 2 passes to get the width of profile required and they are coming out fine on the rails. The only problem left is in the corner. If I run it at 40IPM it's not leaving an acceptable result.

Initially I had the same thought as you, there's no way the CNC will reach that speed and so it's not a relevant factor. Nonetheless when. I slow it way down it using an identical geometry it yields good results.

Right now I am trying to find out from Syntec if there are any parameters in the control that affect the 3 axis motions. And on the other end I am talking with Enroute to see if there's anything we can do to reduce the feed only on the 3 axis moves.

Tom, I can't figure out a way to automate cutting only the prismatic toolpath at a different feed rate from the rest.

I think my next step is to post on a site with more Syntec users and see if anyone there has any insight. I will let you know what I discover.

first question ,is that same problem exactly on all 4 corner?
second: do you have air compesntion cylinder to assist z? if so try reduce the pressure
third: is accl dccl in all 3 axiss are same?
4: there the loop gain parameters in the driver(if its yaskawa its 101,102,103 cheack the value in the 3 axiss and send here
goodluck

Have you reached a resolution to this problem?

BH Davis

Hello All,

Thanks for all the input thus far. I just wanted to give you an update.

I spoke with Syntec and they were pretty helpful. They took a look at a backup of the CNC parameters and suggested reducing the acceleration parameter. By default it's set to 400MS and they told me they have seen machines reduce it to 1500 it 2000. I have experimented a bit and found that reducing it to 2500MS I could get an acceptable corner at a reasonable overall feedrate. Does anyone else have an idea of what acceleration their CNC is set to? Just curious if I am too far out of normal range. My main concern is if it starts to impact other types of operations or increase over all cycle time. I think it should be ok for MDF doors as most of the cutting segments will be long enough to allow the CNC to reach the programmed feedrate.

I have also purchased custom inserts that will allow me to cut the full width of the bevel in 1 pass (I may do 2 passes in the depth but in the same X/Y location) which should eliminate any issues on the rail. I am able to do this because it turns out the customer rarely uses raised panel doors so the larger diameter won't be an issue.

I didn't have any success with getting Enroute to set a separate feedrate for the Z axis moves but I thought that was a bit of a longshot.

In answer to Yakov, yes all 4 corners are consistent. I can look into air pressure on the Z axis. I know it is on a slide so the head drops down on an air cylinder before cutting.

I have received the inserts and will be running more tests on Thursday. I will update you with my findings.

Thanks again.

Richard

A couple points.

First, in Enroute, if I am understanding you correctly, you can set a separate feed rate for Z as vs. X and Y.

SETUP, MACHINE SETUP, DRIVER SPEEDS. The Z-axis feed rate is controlled by the default PLUNGE rate. This is FEED rate though, not ACCELERATION rate.

Second point is that with my old CNT Motion router using WinCNC control software I was able to create an onscreen button in WinCNC that temporarily changed acceleration. I created two custom buttons, one to go to a lower acceleration rate and another to bring it back up to normal. We used the lower acceleration for 3D carving work to make the machine move more smoothly on rapid short distance cuts. Pressing the button changed the rate and popped up a note to restart the software with the new rate.

The lower acceleration rate held in effect until the higher acceleration rate button was pushed. As such we always put a post it note on the screen to remind us to reset the rate when the project was complete.

By far the largest issue for us was the acceleration and X and Y. Z was set to move so slowly by comparison that acceleration was not an issue. So if you want to try seeing if lower feed and acceleration rates are going to help I'd suggest temporarily lowering acceleration and perhaps also Z-axis feed rate.

BH Davis