QCAD.org Forum

Versie:
3.30.1.0 (3.30.1)
Internet:
QCAD.org
Aanmaakdatum:
Jun 18 2024
Revision:
5067327
Qt Versie:
5.13.2
Architectuur:
x86_64
Compiler:
MSVC++ 14.0 (2015)



Hi,
I am trying to mill out a circle 60mm where first a hole is made with a drill 2.5 mm This hole wil come in the middle of the circle ) and then the milling cutter 2.5 mm has to mill out the circle through this hole.
I cannot get the milling cutter to start through the drilled hole.
The milling cutter now starts 1.25 mm on the inside of the circle instead of the middle of the circle..

thanks in advance,

greetings Danny

Typically, the drill hole would be placed at the starting point of the lead-in for the profile toolpath after the profile toolpath has been created. Please elaborate why this is not desirable in your case. Can you attach a screenshot or a DXF file also? Thanks.

Hi,

See attached files

Greetings Danny

Hi,

Your milling cycle is defined as inside.

- Show CAM Toolpath List (GA)
- Edit 'frezen 2.5 mm'
- Set the correct side (and direction)

Or Toolpaths are regenerated automatically or enforce that manually.

Regards,
CVH

How about something like this? The drilling happens at the start of the lead in, the drill toolpath is based on a point entity constructed there.

Hi Andrew,

Thanks, for the 60 mm circle this will work well.

How can i make it into this product, first drilling with 2.5 mm then need milling 2.5 mm.

'Profiel 1'
Set Lead In type 'Quarter Circle' (With 'Normal' it will cut out more than the intended circles)
Adapt drill position
Adapt Lead In radius ... But at some point the Lead In may over-cut again with too small circles.

For 'Profiel 2' there is another problem.
I see the quarter circles being cut at the inside.
Your outer contour is not well defined.

Try to double click on one of the segments, where the selection ends it will not be connected.
Try to merge them to one polyline with OC, it will be logically closed when well defined without gaps ... Without dualities.

Regards,
CVH

Hi CVH,

Thanks, but i still don't see that the mill is going into the drilled hole, before milling ?

First have a look at the new outer contour.
Where the quarter circles where typical 90 degrees they are now about 95 degrees or nearly 100 degrees.
You probably have trimmed them to the larger straight edges disregarding the short edges at those corners.
At the left high quarter circle the 2 slots are disregarded.
These 2.5mm wide slots can not be cut by the newly added profile with a 6mm cutter.

And hardly by the 2.5mm toolpath in the former art because a round cutter can not cut a sharp inside corner.
The minimal interior rounding radii are half the cutter size.

danny10 wrote: ↑

Fri Jun 21, 2024 1:48 pm

Thanks, but i still don't see that the mill is going into the drilled hole, before milling ?

The drilling cycle is independent of your profile cycle.
QCAD will not automatically use the pre-drilled holes as entry positions.
In Andrews example the hole to drill is placed at the start of the Lead-In.
That is what I meant by "Adapt drill position".

Normally a suited router bit can plunge straight down into the material at low FEED.
Although a gentle ramp down into the material is far better for this type of cutters and this can be done at optimal FEED.
Indeed, some end-mills are not capable of doing that an a pre-drilled hole is required.
Then the pre-drilled hole is typically at least somewhat larger than your end-mill.
You may ruin your cutting edges of your mill when it is a tight fit ...
... It is rubbing instead of cutting on the way down but that also depends largely on the type of stock material.


Partial solution:
The only way I see that a Lead-in path can start at the center of the hole and end cutting tangentially at the outer edge is using a hole size related Lead-in that is a semi circle.
Under QCAD/CAM and for a hole of 15.24mm diameter that would be something as a semi circular Lead-in with R=3.81 (=25% )
But for a hole of 6.604mm that would fail ...
... Simply because R=1.651mm and for some reason the entry radius must be larger than the tool (>2.5mm).
Below you can see that it is perfectly feasible and that the radius of the entry path is not 1.651, in green with R=1.026 it is even smaller.

In yellow I represented the cleared area by the cutter and that is fully unrelated to the red Lead-in.
But perfectly related to the green entry path.


For me this is a misconception
There is something wrong with calculated offset paths ...
Seemingly the circular Lead-in is defined as the arc from center mill to the outer edge of the mill (In red).
As if the cutter has no size to start with and ends with a certain radius.
As if the cutter size is gradually compensated from zero to R=2.5mm.
Mimicking G41/42 but a (linear) cutter compensation can never be done in a circular motion.
The motion required going trough the virtual centers is not a simple arc and certainly not supported by all motion controllers that I know of.


Related: https://www.qcad.org/rsforum/viewtopic. ... 724#p44206
For a eighth circle I call it 'donkey ears' and you may discover that it won't be fixed.


You fooled the profile generation with a cutter = 2.499 and Lead-in Radius = 2.500
But that won't do the trick ....
And it is not the whole story because we are missing the cutter path starting at the Lead-in begin and something similar for the Lead-out.
The standard assumptions and Math for the offset are failing here.
The offset path should be a dot, simply plunge and back up with no motions in XY and disregarding a Lead-in/out or overcut.


A hole that is pre-drilled by a 2,5mm drill ... Does that require milling by a 2,5mm mill?

As said, the QCAD/CAM Lead-in radius must be tweaked according the hole size.
There is no one shoe that fits all.
Applicable for hole sizes of over twice the Lead-in radius although it is feasible for 100,00..01%
At some point you may consider drawing the offset path and Lead-in (dotted) yourself as per example dxf and mill on path ...

Regards,
CVH

Hi CVH,
Thanks for your help.
We did it like this:
First setup milling then where the milling starts we drilled a hole.

That works fine for us.


thanks

Greetings Danny

Hi,

I understand the simplicity of your approach Although it is a manual intervention.

May I still point out that the outer contour of test27-6-2024.dxf can not be compared with the initial design in the Test.dxf
The larger circular contours where 90° and ended in line entities indicated in red:
The two slots left high are not fully milled 'open' because the contour is not open at that point.
I have my reserves over plunging into a pre-drilled hole of the same diameter ...
I see no reason to mill out a pre-drilled hole of the same diameter ...

Regards,
CVH

Hi,

The manual intervention is the easyest way to do, now we can mill hundreds pieces the same.
But the two slots we do need to openthem.
Also a new issue came up, the maual change of tools won,t work on this ?
Manually we set Line
1015
2325
2395
2495 with M0.
the machine stops, but the spindle keeps running so we cannot change the tool.


Greetings Danny

danny10 wrote: ↑

Thu Jun 27, 2024 6:41 pm

But the two slots we do need to open them.

This is also a result of trimming the 4 larger arcs piece-wise with the larger straight edges.
Disregarding the short line segments indicated in red above originally found in your initial design in Test.dxf .

You should post unrelated questions as a new topic.
See above forum rules in red.

GCodeOffsetMM.js is based on GCodeMM.js and
GCodeMM.js is based on GCodeBase.js

In GCodeBase.js there is an empty toolFooter block defined.
The two other standard postprocessors files don't overrule that.

Do NOT edit this file. Your changes will be lost when the software is updated or reinstalled.
See script file header.

You need to include a specific toolFooter block for a custom postprocessor based on GCodeOffsetMM.js.
For example called GCodeOffsetMMToolchange.js or GCodeOffsetMMHalt.js.
Remind to also adapt the displayName to something meaningful.

Something as below should do the trick: Regards,
CVH