Pocket path option

Discussions around the CAM Add-On of QCAD.

Moderator: andrew

Forum rules

Always indicate your operating system and QCAD version.

Indicate the post processor used.

Attach drawing files and screenshots.

Post one question per topic.

User avatar
K0nrad
Junior Member
Posts: 23
Joined: Sun Jan 02, 2022 11:59 am

Pocket path option

Post by K0nrad » Mon Jan 03, 2022 9:52 pm

Hello,
I started working with QCAD/CAM relatively recently, mainly for the projects for my CNC machine. Overall, I am very happy about the CAM module. Considering its capabilities, I would like to suggest one more function. It's about generating paths for pocket milling. Currently I do it "by hand" using "Offset with distance" and "Break out Segment" options. It works, however it requires a lot of time and attention from the designer (e.g. precise calculation of the distances vs. the diameter of the bit etc.). Please consider in future version of QCAD/CAM the pocket path tool in CAM module.
Best Regards
Konrad

Windows 10 64-bit
QCADCAM Pro 3.27.1
Postprocessor: grbl mm

CVH
Premier Member
Posts: 1816
Joined: Wed Sep 27, 2017 4:17 pm

Re: Pocket path option

Post by CVH » Tue Jan 04, 2022 7:19 am

Konrad,
this is a known shortcoming.

Have a look at:
https://www.qcad.org/rsforum/viewtopic.php?t=5411

It is not that easy to implement a spiraling milling pocket path.
Like Husky remarked recently: The multi offset method uses a lot of ups & plunge.
And for me the offsets of 'artwork' are not always correct.

Regards,
CVH

User avatar
Husky
Moderator/Drawing Help/Testing
Posts: 4248
Joined: Wed May 11, 2011 9:25 am
Location: USA

Re: Pocket path option

Post by Husky » Tue Jan 04, 2022 10:12 pm

K0nrad wrote:
Mon Jan 03, 2022 9:52 pm
Currently I do it "by hand" using "Offset with distance" and "Break out Segment" options. It works, however it requires a lot of time and attention from the designer (e.g. precise calculation of the distances vs. the diameter of the bit etc.).
Yes I agree - It would be nice to have a decent pocket tool!
K0nrad wrote:
Mon Jan 03, 2022 9:52 pm
Currently I do it "by hand" using "Offset with distance" and "Break out Segment" options. It works, however it requires a lot of time and attention from the designer (e.g. precise calculation of the distances vs. the diameter of the bit etc.).
I'm planing to put in a Feature or Scripts/Plug-in/ Add-on request. I'm pretty sure my pocket design is pretty much close to your design but may I ask you to post your solution as a dxf/screenshot? On that way I can consider more needed facts for a tool request. Thanks.
Work smart, not hard: QCad Pro

If a thread is considered as "solved" please change the title of the first post to "[solved] Title...". Thanks!

CVH
Premier Member
Posts: 1816
Joined: Wed Sep 27, 2017 4:17 pm

Re: Pocket path option

Post by CVH » Wed Jan 05, 2022 8:06 am

Husky wrote:
Tue Jan 04, 2022 10:12 pm
I'm planing to put in a Feature or Scripts/Plug-in/ Add-on request.
Odd, but indeed the search term 'pocket' returns no results on Bug Tracker. :?

It does return 35 matches on the forum going back to 2014.
Mostly it all boils down to the advice of using multiple offsets.

https://www.qcad.org/rsforum/viewtopic.php?t=2601
Would be a solution for softer materials like foam or MDF.
On harder stuff one should keep the chip load steady at near optimal cut.

As engraver on metals I won't even consider:
https://www.qcad.org/rsforum/viewtopic. ... 977#p35827
There it swaps from conventional to climb milling and back.
The same is true for Zig Zag: https://www.qcad.org/rsforum/viewtopic.php?t=8023
Although, again fine for softer materials. :wink:
Husky wrote:
Tue Jan 04, 2022 10:12 pm
On that way I can consider more needed facts for a tool request.
  • - Cutter size; Step size; Finish pass step size; Step size in Z; Finish pass step size in Z.
    - Modes: Spiral in/outwards; Zig Zag & angle.
    - Methods: Conventional (up) or climb (down) milling.
    - Optional forced conventional for finish pass.
    - Plunge, spiral down or slope in Z with re-cut.
    - Cutter path rounding for continuous motion.
    (Minimum radius depends on max. accelerations)
    - DogBone fillets or overcutting hard corners.
    - Warning when pocket is not fully cut at too steep path angles.
    - Warning when outer boundary can't be cut with given cutter size.
    - ...
Regards,
CVH

User avatar
K0nrad
Junior Member
Posts: 23
Joined: Sun Jan 02, 2022 11:59 am

Re: Pocket path option

Post by K0nrad » Thu Jan 13, 2022 7:16 pm

Hi,
Here is a simple example of manual pocket design using QCAD including dxf project and a photo of the result. A more accurate result (but longer milling time) I obtained for for paths perpendicular to the length of the cut detail. With "manual" design of the g-code for the pocket, there are two important things are: the order of the individual steps and the distance between the paths regarding the bit diameter. It seems to me that if QCAD had an option for filling closed areas with polylines of different course (spiral, straight, zig-zag etc.) taking into account the given distance from the area boundary, generating a g-code for pockets would be very easy.
https://drive.google.com/file/d/1ma1VO0 ... sp=sharing
https://drive.google.com/file/d/11QensH ... sp=sharing

User avatar
Husky
Moderator/Drawing Help/Testing
Posts: 4248
Joined: Wed May 11, 2011 9:25 am
Location: USA

Re: Pocket path option

Post by Husky » Fri Jan 14, 2022 3:42 am

K0nrad wrote:
Thu Jan 13, 2022 7:16 pm
Hi,
Here is a simple example of manual pocket design using QCAD including dxf project and a photo of the result.
Great example - thanks for that!

I noticed your effort to create the pocket path. I'm right now playing with your example file - may I ask you how long it took you to create that path with the "Offset with distance" and the "Break out Segment" tool? And ... the theoretically time for CNC milling is around 1:43 h?
Work smart, not hard: QCad Pro

If a thread is considered as "solved" please change the title of the first post to "[solved] Title...". Thanks!

User avatar
K0nrad
Junior Member
Posts: 23
Joined: Sun Jan 02, 2022 11:59 am

Re: Pocket path option

Post by K0nrad » Fri Jan 14, 2022 9:46 am

The longest part of the design was to figure out what drawing should be like :D Then it didn't take much time to prepare the drawing itself. For pocket lines preparation, I used additional, single auxiliary lines (option "offset with distance") to determine the distance between the pocket lines (correction due to the bit diameter) and the border of the part shape (these auxiliary lines were later removed). All pocket lines were also created using "offset with distance". Then I removed unwanted parts of the pocket lines by using the "Break out Segment" option. More attention is needed for milling sequence planning. The machining time for both details was about 1h 50min. And here I see another optimization opportunities. The time could be significantly reduced if "Reverse Milling" option would be available when several passes are required for the same path (for open shapes/paths, at least). QCAD, currently, after reaching the end of the path, moves bit up, returns to the beginning of the path and then starts milling again. It doubles the milling time.

CVH
Premier Member
Posts: 1816
Joined: Wed Sep 27, 2017 4:17 pm

Re: Pocket path option

Post by CVH » Fri Jan 14, 2022 1:20 pm

K0nrad wrote:
Fri Jan 14, 2022 9:46 am
The time could be significantly reduced if "Reverse Milling ..."
One doesn't mix conventional (up) or climb (down) milling by default.
That should be a fixed choice given material, cutter type and the robustness of the machine.
I agree that pine is a soft material but the milling method also has an influence on the finish.

I was in the process to pull your design through my CAM included in my driver soft.
Simply to estimate the milling time when using pocketing.
That would be some copy/paste of contours, save as dxf, 3d party CAM, run simulation.
With just 8 contours the preparation would take about 15 min.
What I don't understand is that the outer contour of the clamps is slanted at 0.01478287 degrees.
While the rest is plain horizontal/vertical.
Disregarding the odd overall length and the odd distance between both and a minute horizontal shift.
It then took somewhat longer to 'redraw' it. :wink:
clamps1aCVH.dxf
(106.3 KiB) Downloaded 80 times

Setting up the the 3 CAM profiles and simulation only takes half a minute each.
- Pocketing 9.0mm deep Zstep2.0 Stepover1.8 (=60%!) Finish 0.4 F700: 33min 45s
- Pocketing the slot 9.2mm deeper Zstep2.0 Stepover1.8 Finish 0.4 F800: 9min 04s
- Cut Out Outside 9.2mm deeper with bridges Zstep2.0 F700: 6min 03s
Total running time: 48 min 52s

The first profile looks like this: blue = milling at Feedrate or plunging, red = traversing
ClampPocket1.png
ClampPocket1.png (127.44 KiB) Viewed 2577 times

Optimization should now rather focus on proper chip load, Feed & Speed.
For a 2 flute cutter d3mm softwood chip 0.1-0.15 at 10000rpm the Feed should be between F2000 and F3000.
That would turn out to about 3x faster or a running time less than 20min. :wink:

Regards,
CVH

User avatar
K0nrad
Junior Member
Posts: 23
Joined: Sun Jan 02, 2022 11:59 am

Re: Pocket path option

Post by K0nrad » Fri Jan 14, 2022 3:02 pm

Thank you for your detailed analysis of my project. Very helpful. I fully agree that milling direction should not be mixed by default. However, in this particular case it would help :D. For the software that have the option of generating paths for pockets it is probably unnecessary, because the g-code generation algorithm usually optimizes the path of the bit. What software did you use to prepare your version of the project? I would like to have similar possibility in QCAD Pro.
Best Regards,
Konrad

CVH
Premier Member
Posts: 1816
Joined: Wed Sep 27, 2017 4:17 pm

Re: Pocket path option

Post by CVH » Fri Jan 14, 2022 3:58 pm

K0nrad wrote:
Fri Jan 14, 2022 3:02 pm
I would like to have similar possibility in QCAD Pro.
In QCAD/CAM, yes, me too. :?

I referred to it in my PM to you.
See: https://www.qcad.org/rsforum/viewtopic.php?t=7415
Only for a Windows platform. :(
From contours to G-code in under 5 minutes ... :lol:

Off course it only supports Eding CNC boards like I have, it is build in the driver soft itself.
Here I used it to create the Zig-Zag at an angle in a few clicks and setting the required parameters:
https://www.qcad.org/rsforum/viewtopic. ... 423#p31418
Pocketing at Z0.0, one pass, save G-code and imported the G-code back with QCAD/CAM.
QCAD/CAM can now mill 'on path' using any included or custom postprocessor.

It is just one example on how to circumvent shortcommings and dodge huge fees, there are many little (free) tools out there.

Regards,
CVH

User avatar
Husky
Moderator/Drawing Help/Testing
Posts: 4248
Joined: Wed May 11, 2011 9:25 am
Location: USA

Re: Pocket path option

Post by Husky » Sat Jan 15, 2022 9:12 am

K0nrad wrote:
Fri Jan 14, 2022 3:02 pm
I would like to have similar possibility in QCAD Pro.
Let see ...
Your G-Code has 5629 lines, your machining time is for both details about 1h 50min. Correct?

After playing a bit with the project ...
... my G-Code has now 792 lines and the machining for both details would take around 37 minutes. And yes, I used ONLY QCAD Pro tools to prepare the drawing and CAM. I'm sure you noticed that the Pocket style is a kind of a "Outside the Box" solution but it works flawless. And it is fast - the design for the Pocket took around 30 seconds.

G-Code.gif
G-Code.gif (1001.74 KiB) Viewed 2513 times
Work smart, not hard: QCad Pro

If a thread is considered as "solved" please change the title of the first post to "[solved] Title...". Thanks!

User avatar
K0nrad
Junior Member
Posts: 23
Joined: Sun Jan 02, 2022 11:59 am

Re: Pocket path option

Post by K0nrad » Sat Jan 15, 2022 5:22 pm

Hi,
I started to modify my approach to pocket milling in this project because I noticed it is actually too long. However, your solution is even better - thanks a lot for this suggestion.
Regards,
Konrad

CVH
Premier Member
Posts: 1816
Joined: Wed Sep 27, 2017 4:17 pm

Re: Pocket path option

Post by CVH » Sun Jan 16, 2022 7:32 am

I have my doubts whether everything is cleared here:
Not cleared.png
Not cleared.png (39.4 KiB) Viewed 2435 times

Cutting a slot 7mm wide with a 3mm cutters with offset inside leaves 1mm material standing.
This can be a dangerous habit, pocketing 7mm wide is advised.

Cutting out 18.2mm deep with a 3mm cutter in full cut traveling trough a 3mm wide groove may clog your cutter.
It should be cleared somewhat wider so the chips can be removed sideways from the cutter.

A finish pass is another advisable approach.

All that take 11 minutes longer, there is no magic in material removal rate given F700/800; S10000; Stepover 60%; Zstep 2.00.

Regards,
CVH

User avatar
Husky
Moderator/Drawing Help/Testing
Posts: 4248
Joined: Wed May 11, 2011 9:25 am
Location: USA

Re: Pocket path option

Post by Husky » Sun Jan 16, 2022 8:45 am

CVH wrote:
Sun Jan 16, 2022 7:32 am
I have my doubts whether everything is cleared here:
Feel free to doubt my design. I have the drawing which proofs it will clear the area perfectly.
CVH wrote:
Sun Jan 16, 2022 7:32 am
Cutting a slot 7mm wide with a 3mm cutters with offset inside leaves 1mm material standing.
This can be a dangerous habit, pocketing 7mm wide is advised.
Dangerous habit to leave a 9.2 x 1 mm wood steg which is considered as waste material? LOL. I don't share your concern! Pocketing would be an absolute overkill.
CVH wrote:
Sun Jan 16, 2022 7:32 am
Cutting out 18.2mm deep with a 3mm cutter in full cut traveling trough a 3mm wide groove may clog your cutter.
It should be cleared somewhat wider so the chips can be removed sideways from the cutter.
Well, it plunge 9.2 mm into the material and not 18.2! What is half of the first here presented solution. However - God bless the invention of vacuum dust collectors what should eliminate your clogging concern.
Work smart, not hard: QCad Pro

If a thread is considered as "solved" please change the title of the first post to "[solved] Title...". Thanks!

CVH
Premier Member
Posts: 1816
Joined: Wed Sep 27, 2017 4:17 pm

Re: Pocket path option

Post by CVH » Sun Jan 16, 2022 10:08 am

A) You didn't provide a drawing nor a proof of concept.
B) Part of the clamp block is grove slotted 18.2 deep.
C) Dust removal or flushing liquids only efficiently removes chips brought up to the surface.
D) I really hope for you that nothing left standing freely nor any piece of broken cutter is ever projected in your direction.

About every CAM handles chip load calculations to set up Feed and Speed.
These days that is dynamically adapted to the actual position in the path.
There is a lot to gain in project milling time and cutter standing time, both are human labor intensive.
Please study that part of the CNC milling process in detail, you will end up with pocketing.

There you don't want advise from a trained/experienced machinist, I rest my case.
I then also fully agree that proper CNC practice is completely OFF-topic for drawing under QCAD.
I'll use my 8 contours, my CNC driver does the rest.

Regards,
CVH

Post Reply

Return to “QCAD/CAM”