Feature request: Multiple horizontal passes on Profile/Contour?

[roivai]

Hi,

I don't know if I'm the only one, but being able to create profiles/contours with multiple passes on horizontal direction would be very beneficial. At least when milling crappy aluminium with crappy tools, it is the only way to get deep parts cut out. This is because running tool-width slots without proper coolant the chip evacuation will eventually fail and the end result will be a molten glob of aluminium and a disappointment. But if the slot is cut even 1mm wider than the tool, things usually work for me at least.

I've usually hacked this by creating some dummy shapes around the desired contour and created a pocket for that. But that is rather annoying. Also, I've been checking on tutorials on other CAM systems (Fusion360 mostly) and there this problem is usually handled by defining the stock and then using some cool adaptive algorithm to remove all the material on the outside of the part. This would of course be the best way, but as we might be rather far from being able to do that, I just thought that it might be easy to add possibility to create multiple passes for profiles/contours. The very little I understand about the new Path.Area, this shouldn't be too difficult? In practice, I think the best way would be to ask for desired width of the cut and then if the cut is wider than the tool, it would be done with multiple passes. And please note that this is different than the Finish Pass option there is already, as for the chip evacuation to improve, the extra pass needs to be done separately for each Z-step.

Am I the only one who would find this beneficial? @sliptonic any idea if it would be difficult to implement? If answer to either of those is yes, then this should probably be ignored..

[herbk]

Hi roiwai,

Am I the only one who would find this beneficial?

Some time before i asked for it to...

[mlampert]

Hi roiwai,

Am I the only one who would find this beneficial?

Some time before i asked for it to...

Are you asking for it because we currently don't consider stock or do you actually want to make a profile op with a wider cut than the tool regardless?

[Konstantin]

As I understand, the Idea was that for horizontal faces you should use Face milling operation, and then make finishing Profiling contour. But problem is that Face milling does not work right. I attached example.

[bill]

I don't know if I'm the only one, but being able to create profiles/contours with multiple passes on horizontal direction would be very beneficial. At least when milling crappy aluminium with crappy tools, it is the only way to get deep parts cut out. This is because running tool-width slots without proper coolant the chip evacuation will eventually fail and the end result will be a molten glob of aluminium and a disappointment. But if the slot is cut even 1mm wider than the tool, things usually work for me at least.

This is what "Clear to Target" is all about! Clear to Target ( BBox, Stock perimeter, OFFSET, projection, and on and on...)

The very little I understand about the new Path.Area, this shouldn't be too difficult? In practice, I think the best way would be to ask for desired width of the cut and then

You are correct sir; it is a piece of cake to accomplish what you are asking! I have already hacked together (from realthunders Path.Area) enough to satisfy my needs since no one was interested.

The selected operation, i.e., profile, contour, etc. is one of the bounds, the Target is the other, and essentially a pocket operation is performed to clear the material.

This is more useful than spending a whole lot of time honking-up the tool tables with impractical/unrealistic characteristics; Keep It Simple Stupido

BEWARE of the Bounding Box; it seems to have trapped several people at this point.

[herbk]

Hi Markus,

Hi roiwai,

Am I the only one who would find this beneficial?

Some time before i asked for it to...

Are you asking for it because we currently don't consider stock or do you actually want to make a profile op with a wider cut than the tool regardless?

my first question about it was sometime last year (if i remember right), for same reason as roivai explained: On some materials its good to have more space for the chips.

I don't need it frequently, but if, i use a workarund: First i make a contour path with a bigger tool diameter, then a path with the tool diameter which is in the machine.

[mlampert]

You are correct sir; it is a piece of cake to accomplish what you are asking! I have already hacked together (from realthunders Path.Area) enough to satisfy my needs since no one was interested.

The selected operation, i.e., profile, contour, etc. is one of the bounds, the Target is the other, and essentially a pocket operation is performed to clear the material.

Care to submit a PR?

[sliptonic]

Am I the only one who would find this beneficial? @sliptonic any idea if it would be difficult to implement? If answer to either of those is yes, then this should probably be ignored..

The answer, of course, is; It depends.

It would be easy to add a 'kerf width' property which defaults to the tool diameter. Then the profile/contour operations could use it to build an additional offset at each layer.

However, I expect that the very next thing we would hear would be a request to have a different number of step-downs for the two off-sets. For example, it would be nice to do 3 steps down on the primary profile, then do 1 more pass at the last depth to widen the kerf. Then three more steps and another widening pass.

If we're going to want this kind of control, then I think we need to have a different kind of operation or else a dress-up. Either of those would be more difficult.

I think this is a good feature but let's do it right. Let's add a feature request to mantis linking to this thread and continue the discussion.

[VVilhelnn]

Hi everyone,

I am also very interested on this feature. Is this in the ToDOs list and if not, where do I add my extra vote to make it happen.

From folks who have work around this without the feature... What is your solutions to the problem specially when we have non regular boxes or shapes. I saw @bill reply, but I didn't quite get how that operation was done to basically create a pocket around an object (outside) and just at the part edge not entire bondy box, if any one know please more details

Most of my problems happen at the last step down when cutting through the material (aluminium) to waste board. My current NON-perfect solution is to create two profiles one with extra offset of half of the tool and stop just one millimeter before cutting through material. Then the final pass, which will have room for all the chips. This usually works for less than 12.7mm anything taller and might need to do 3 passes.

if I could just mareg those two profiles into one. outside pass, inside pass, outside pass, inside pass, etc, etc... I don't think I need the n times outside then n time inside just one and one.

I was considering if there there a way to create a macro-line in python to take an existing profile operation and create a new operation with the two passes per step down. Of Course outside first (or away from the part) then inside (or closer to the part), inside/outside from outside profiles PoVs. I guess this will look more like a dress up operation.

Thanks for any information I would love to stop doing all of the extra work manually, At the beginning I also used to create extra parts (jibs) jus so I can use a pocket operation in profile mode around the part, but it gets annoying fast thus the two profiles for now.

I could help coding if some one can provide a good guide/crash course on FreeCAD/Path "hello world" with manipulating other operations in document cheash curse.

-Wilhelm

[RatonLaveur]

Have you tried an adaptive profiling? or an adaptive clearing from outside?