QCAD.org Forum

Good morning.

OK I have learned a lot about designing in QCAD, but I have a problem I need an answer or fix for.

I am running Windows 10, using the current QCAD/CAM version, with a Genmutsu 4030 PROVeXL 4030 V2.

I am design instrument panels for experimental aircraft. After I design the panel, I then run CAM to generate the GCode. When I get to the Side/Direction, on the instrument holes, I change to Inside, and Conventional/Right. When it generates the tool path, I get this. Notice the lines in the red circle, and this happens on all of the inside cuts. On Lead in Type, I put Normal, and Lead in Length, I put .125, half the size of my mill bit.
Now, when I do a practice cut, it cuts on the design line, not the offset line.

Making a few changes, I also get this problem. The first photo is an instrument hole I designed, when I put the lead length of zero, it cuts on the line, but when I add say, 1, it shows on the Visualizer the second photo.
What am I doing wrong, and how can I fix it? For an old guy, learning QCAD has been pretty easy, but this is something I need to get right, without having to offset all the instrument holes to compensate the instrument drawings to cut where I need it to cut.

Thank you in advance for your help.

Brian

I would recommend to make sure all contours are closed polylines and to move the start point to a suitable position that can host the lead in / lead out movements.

Please refer to our QCAD/CAM tutorial for an example:

https://www.qcad.org/en/tutorial-qcad-cam

-> Creation, Preparation and Selection of the Geometry, Step 2

Thanks.

Are you referring to the second problem? I will try that tonight, and follow up if that doesn’t work.

Still looking for fix of the first problem.

For both problems (and all contours in general) the starting position needs to be suitable for the lead in / lead out. This is usually at the center of a longer element for inside cutting or for outside cutting at a corner. If I understand your screenshots correctly, this is the problem for both situations.

Andrew,

Thank you very much. I think I have figured it out. You were a big help.

That Tutorial was a big help also.

Tomorrow, I will test it all out on the CNC.

Brian

Hi,

Hard to tell without a QCAD/CAM file but EB8F7781... and DCEB9812... doesn't seems right disregarding the Lead in/out.
If possible please attach a CAM DXF so we can help you more efficiently.

We typically design the required hole as the outer edge to be milled.
The central offset path of the mill is then at the inside.

The path encircled at the right-high in DCEB9812... would not produce the contour seen in EB8F7781...
Important here is that the mill radius is less than the radius of the smaller inner rounding.

I also think that you can not use the 'Normal' Lead in/out mode when milling holes.
Not really 'Normal' or the opposite of 'Tangentially' but at least this includes a motion reversal.
Neater would be when the mill approaches the intended path gradually from the inside.

At best as far from a 'corner' feature as possible like pointed out by Andrew.
Preferable at a straight edge but that is not really possible here.

Regards,
CVH

CVH

OK, Here is one that is more pressing. It is a panel I am working on. I think if I can get this figured out, I should get the other one figured out. I just cut it on a piece of wood, as cheaper to test, then on aluminum.

Everything went well, except all the inner boxes, which are red, and the outside edge, which is green, cut center on the line, so each is .125' bigger than I want.

Per Andrews point. I clicked on the lines to create polylines, then I was able to move the start points in the middle of the straight lines in the boxes. As you see in the DXF files you will see the cut side on the inside of the red lines, and the outside of the green lines, but it is still cutting on the center of the lines.
FYI, I am using drills to drill the small holes, the yellow and Orange, and a mill to cut the boxes, red, and the outside, green.

Hi,

Sorry to say but I can only detect 2 drill paths ... Sort of, because their type is reported to be a 'Profile'.
Beside that, you are using a metric post processor for a drawing in inch with a custom metric paper size of 8.5 by 11mm.
Not that this last matters.

To be honest, I don't use the CAM addon of QCAD, my controller has a build-in CAM and accepts DXF files in direct.
Perhaps it is simply a limitation of a QCAD/CAM trial version.


Note that the green rectangular shape is about 7.25 by 11 units but it is not really a rectangle.
Horizontal lines are not equal and near but not at an angle of 360 or 0 degrees.
The same for the vertical lines but then near and not at an angle of 270 degrees.

The top red shape suffers from similar faults and only that red shape.
Only the lower right red rectangle is a polyline but still has the start point in a corner.

Your drawing origin is (nearly) bottom center of the 'distorted' shape in green.
QCAD has no relative origin feature, meaning that you must zero your CNC setup at that position on the substrate.
Best done with zeroing first in XY with the cutter a little above the substrate.
Then in Z ... Top of your material is Zzero.

Your setup is a manual tool changer.
Also meaning that you must re-zero your Z-axis after a tool change to compensate for the tool length.


You are using a generic metric post processor that supports G41/42 modes or cutter radius compensation: G-code (G41/42) [mm].
If I look up the Genmitsu PROVerXL 4030 V2 then I read that it is a GRBL v1.1h-Based controller.
GRBL does not support G41/42 as far as I know, only G40 to turn these modes off.

True, with G41/42 support we export the required contour.
It is then the controller that ensures for a left or right offset trajectory.
For example G41 P2 would compensate the cutter trajectory 2 units to the left seen in the direction of the cutter motion.
If these modes are not supported the processing should fail with a warning, ignoring these codes may look like milling 'on the contour'.

I would advise to use the GRBL (offset) [mm] or [in] post processor.
Not aware if this the best suited for your setup, as QCAD post processors are incredibly versatile and may require custom adjustments.
It is then QCAD/CAM that generates the offset path.
Select inside for holes and outside for the exterior contour (After fixing ).


As direction we can use Conventional or Climb milling.
See pros and cons on for example this link.

Routing is more related to groove cutting, your milling tool is engaged with the material for about 180 degrees.
Conventional/Climb is then of less importance but depending your setup one side of the groove will have a neater finish.
In this price range I don't expect a robust or very stiff machine.
Your best option is then a pre-cut followed by a finishing pass of less than 1/4 of the tool diameter.
Use the best solution of Conventional vs Climb cutting for finishing depending your setup, the material type, the mill type and so on.


For now QCAD/CAM supports 2 types of tool paths: Profiling or Drilling.
Generate a individual Drilling toolpath for the yellow and the orange layer.
Drill diameter and the circles on the yellow layer are a match: 0.1495in.
On your orange layer you have holes with: 0.0625, 0.096 and the oddball 0.11954358220110403 diameter.
All drilled with diameter 0.098in.

Convert all contours to polylines (OC) and set a good start point (OR)

Generate a Profiling toolpath for the red layer as cutting inside, direction as per above.
Generate another Profiling toolpath for the green shape cutting outside.
Choose a Lead in/out and overcut what suits you, the defaults of 5 units = inch are too large.


Without a vacuum table or a sticky surface, you have to hold down the excess material.
When a contour is almost cut, this excess can shift and the cutter can grab and throw it away.
Tool breakage is then the least of your worries ...

Extra clamps are usually not an option as they are in the way of the cutter path.
We can add TABs or short uncut portions that bridge the gap of the groove.
Efficiently retaining the left over.
Afterwards you need to cut that out manually or simply break it out.
Other solutions include for example to fix it down with at least 2 screws.
Double sided tape is not really reliable for this purpose and the thickness is not uniform.

Regards,
CVH

Here I used: G-code (offset) [mm]; As polyline, start is top middle; Inside; Climb or CCW here; Quarter Circle 0.2in Lead in/out; Overcut 0.3in
Tool characteristics, Cutting Depths and Passes at your discretion.
Don't overdo it in aluminium, maximum deep groove cutting is typically 2-3 times your cutter diameter but soft aluminium is sticky.
Best done with a Cutting Fluid but your setup is intended for dry use only.

Feedrate is then also in inches per minute: 200in or 5080mm per minute, 5000mm/min is the reported max FEED.
Depending your cutter type, plunging must be done gently, say at 10-20% FEED
A mill is not really like a drill what is intended to go straight down.
The surface of aluminium is oxidized and that is a ceramic.

In all cases we should use TABs to retain the left over


Regards,
CVH

CVH,

Thank you for all those inputs. I printed up your post, and I will redo that panel, with your corrections. I will post an update when I figured it out.

I am still learning, but in the past, I just design it, and send the DXF file to Send Cut Send, and a week later I have the part. The worse part about it, is I live 3.2 miles from them, and have to wait, two to three days extra to get the part from them, as they wont let me pick it up.

Again thank you for your help, and will let you know what happens.

Brian

CVH,

OK, I redid the whole panel, and used the GRBL Offset mm, and keep the whole design in MM, and tabs.

It seems to look correct in Candle now, including the inside and outside cuts, and it matches your example.

In the morning, I will be doing a practice cut in wood, and if it is all correct, I will do it in aluminum. Then I will be doing the other pieces needed to finish up the panel.

I want to thank you very much for all your help in this matter. I am learning a lot.

Just for my own info, which CNC do you have that has the CAM built into the controller?

Brian

Brian,
Glad that it already looks more OK.

Next step is to become a trained CNC machinist.
Expect a learning curve with the occasional failures and take the time to build up experience with your setup.
Search online and learn the in and outs of CNC machining.
Ask questions when you are stuck.

Please re-read the top paragraph in red of the QCAD/CAM tutorial carefully.
Wear at least a safety goggles, you have but one set of eyes.
Even a desktop setup should have a big red and easy to reach emergency button.

A piece of a 4mm tungsten engraving bit embedded in my Crawford garage door reminds me every day how dangerous it can be.
I assumed everything was perfectly zeroed but somehow it was not.
At 60k RPM it plunged way too far down and the tool scattered on impact, projecting fragments in all directions.
Afterwards I stopped assuming, verifying things more than once.


Before a test in wood I would advise 'cutting air'.
Zero your setup in Z so high that the cutter can never engage with the material.
For that my controller soft lists the extends of the expected motions in XYZ on loading an nc-file.

skyking wrote: ↑

Fri Apr 25, 2025 5:51 am

Just for my own info, which CNC do you have that has the CAM built into the controller?

Refer to this forum topic
I knew Bert Eding personally but I think that he retired.
He worked for some major firms, like Philips, in the R&D and CNC branch before starting his own firm.

When considered as solved please add [SOLVED] to the title of your initial post by editing it.

Regards,
CVH