About the diameter of the tool and the amount of cutting

Here's the place for discussion related to CAM/CNC and the development of the Path module.
Forum rules
Be nice to others! Respect the FreeCAD code of conduct!
Post Reply
jack9603301
Posts: 21
Joined: Tue Oct 12, 2021 6:10 pm

About the diameter of the tool and the amount of cutting

Post by jack9603301 »

I want to know why freecad sets the tool radius of the tool magazine to decrease by default? We usually refer to this setting as the cutting capacity for a single pass. The correct setting of the cutting amount is closely related to the rigidity of the mechanical equipment, the tool, the programming and the technical level and habits of the operator, the material to be processed and the processing accuracy requirements. It is extremely dangerous and unacceptable to confuse it with tool diameter.
Does anyone in the community have an explanation for this issue? Because I'm really curious. Of course, I know this setting can be modified!
Anyway, for most of freecad's features and cams, the community has done a great job. It seems freecad is the only best option
User avatar
sliptonic
Veteran
Posts: 3457
Joined: Tue Oct 25, 2011 10:46 pm
Location: Columbia, Missouri
Contact:

Re: About the diameter of the tool and the amount of cutting

Post by sliptonic »

The simple answer to your question is that it is that way because most of the developers, myself included, are not CNC / CAM professionals. The Path workbench was started by hobbyists and has only recently started attracting professional/commercial users because it's just now maturing to that point.

Of course we would like to continue this process and we welcome input. If you'd like to contribute your expertise on CNC/CAM best practices, it will be welcome. Let me return the favor and offer expertise on contributing to a software project:

Please try to frame your questions and comments using terminology of the FreeCAD/Path project whenever possible. For example you refer to "tool magazine" but this isn't a Path term so it's confusing. Do you mean the tool library? Something about the Tool Controller? The tool changer on the physical machine?

Be careful with phrases like "I want to know..." and "Does anyone in the community have an explanation for this issue?" It may be unintentional but those come across as accusing. They put the focus on explaining and justifying rather than improving the software.

Finally, a picture is worth a thousand words. Add a screenshot and highlight what you're referring to. Link to documentation or videos explaining concepts that might be unfamiliar to us. If you're proposing a change to the UI, mock it up or sketch it on a piece of paper. Anything is better than pure text to make ideas clear.
jack9603301
Posts: 21
Joined: Tue Oct 12, 2021 6:10 pm

Re: About the diameter of the tool and the amount of cutting

Post by jack9603301 »

sliptonic wrote: Thu May 26, 2022 1:44 pm The simple answer to your question is that it is that way because most of the developers, myself included, are not CNC / CAM professionals. The Path workbench was started by hobbyists and has only recently started attracting professional/commercial users because it's just now maturing to that point.

Of course we would like to continue this process and we welcome input. If you'd like to contribute your expertise on CNC/CAM best practices, it will be welcome. Let me return the favor and offer expertise on contributing to a software project:

Please try to frame your questions and comments using terminology of the FreeCAD/Path project whenever possible. For example you refer to "tool magazine" but this isn't a Path term so it's confusing. Do you mean the tool library? Something about the Tool Controller? The tool changer on the physical machine?

Be careful with phrases like "I want to know..." and "Does anyone in the community have an explanation for this issue?" It may be unintentional but those come across as accusing. They put the focus on explaining and justifying rather than improving the software.

Finally, a picture is worth a thousand words. Add a screenshot and highlight what you're referring to. Link to documentation or videos explaining concepts that might be unfamiliar to us. If you're proposing a change to the UI, mock it up or sketch it on a piece of paper. Anything is better than pure text to make ideas clear.
I think even CNC amateurs (including me) should learn relevant professional knowledge (at least common sense) in their hobby field. The step down of machining is not necessarily equal to the diameter of the tool, their theoretical decline The maximum value actually depends on the range of parameters allowed by the tool (of course, larger diameters usually allow deeper milling), but we should also recognize that different people, equipment, and materials allow a single step down value It is uncertain. In a sense, it is safer to be small (especially for novices without any processing experience), but at the same time it will prolong the processing time (of course, this should also be selected according to the processing requirements), Based on this, it is not hard for us to see, even for amateurs, that simply setting the default value of step down to the tool diameter is a mistake, of course, we admit that all software defaults should assume that there may be problems and checking. So, I just want the community to think about this, I don't know why, and whose proposal was in the first place: we should set the default value of step down to be the tool diameter. The initial idea to give a similar proposal might just simply not be able to find a default value that can be provided, so temporarily replace it with the tool diameter; or just not knowing it at the time and finding the error later, anyway, it's a bug, no need Doubt that, although perhaps almost all customers will check/adjust their defaults (they assume some defaults are clearly wrong or even completely wrong) in order to get the CAM designed toolpaths to fit their requirements, but obviously if There is a possibility to improve this, so great, I see no reason to explain this further to prevent misreading by beginners (even if it is temporarily impossible to modify, at least the documentation provides a warning, although most people quickly find out in practice This problem, CNC also has a certain risk, they have no reason to be careless)

Of course, maybe my point of view may also be wrong, I'm not an infallible god, but please don't misread it, for example, in the case of guarantee requirements, of course relatively bigger is better (because it's fast), but The step of the tool is related to the rigidity of the tool, the machine tool and the material, and it is an obvious mistake to simply make it equal to the diameter of the tool. For operators without any experience, it is safer to learn from small steps and try them (processing is not as fast as possible, sometimes it only consumes time if it is slow, but if it is fast, safety accidents or quality degradation may occur, especially are inexperienced operators, like you said hobbyists, they may take some time to find the right parameters).
Screenshot_20220526_224034.png
Screenshot_20220526_224034.png (214.54 KiB) Viewed 1383 times
User avatar
sliptonic
Veteran
Posts: 3457
Joined: Tue Oct 25, 2011 10:46 pm
Location: Columbia, Missouri
Contact:

Re: About the diameter of the tool and the amount of cutting

Post by sliptonic »

jack9603301 wrote: Thu May 26, 2022 2:28 pm I think even CNC amateurs (including me) should learn relevant professional knowledge (at least common sense) in their hobby field.
Agreed. But there's only 24 hours in a day so it's impossible to be expert in everything. The nature of software development is that you have to be a jack-of-all-trades. The pool of software developers who also are hobby machinists is pretty small. Even smaller, those who have access to professional equipment with tool changers, 5th axis, lasers, etc, etc. Now narrow THAT group down to those who also understand human systems well enough to design an efficient user-interface.

Generally speaking, software developers appreciate what they don't know. They respect the expertise of others and rely on experts to guide them. They design for many different use-cases. Non-programmers, on the other hand, usually assume all users are just like them and attribute unexpected software behavior to a bug, bad design, or incompetence.

Enough of that. Back to Path!
The step down of machining is not necessarily equal to the diameter of the tool, ...
Right. So you have four choices:
1) Take a guess. (what we do now).
What's a reasonable guess at a step-down value? Well, that obviously depends. You can't assume users are cutting metal. We have a lot of woodworkers here and for a CNC router, a 1xDiameter step-down is entirely reasonable. For a milling machine cutting aluminum, maybe not. For inconel or some other exotic nickel based alloy, almost certainly not.

2) Make SMARTER guesses.
This just kicks the can down the road. Now instead of guessing what step-down to use, we're guessing what material to use, or what kind of machine you have, or how experienced the user is, or how rigid your tool might be. It's the same problem.

3) Take NO guess. Leave it blank and force the user to set something.
This is extremely confusing to new users. The rule-of-thumb is that the system should provide some feedback and let the user improve the output rather than providing nothing until the user gives everything required. Step-down is just the beginning. There's also step-over, feed rate, spindle speed, etc. Should we refuse to generate ANY toolpath until the user has configured ALL the variables?

4) Detect that the user is using the default value and warn them.
Actually we do this now. The Path Sanity report checks if the tool controller is using default values and adds a 'squawk'. We could do the same thing for default step-down and step-over. The problem with this approach is that you're either annoying the user with warnings or you're relying on them to check the sanity report. The users who are least likely to do this are the ones who probably should.

Assuming we're still going to make a guess. Perhaps we should make a more conservative guess -- perhaps 1/2 or 1/4 of the tool diameter. Easy enough but it has two side effects. First, as you noted, the toolpaths take longer to generate. Worse yet, the toolpath visualization becomes very dense -lots of green lines. It's harder for the user to see what's going on. The step-down is safer but the risk of an undetected collision is greater.

So, if you know nothing about the material, machine, tool, or user, what's the best step-down guess to take? What's the best trade-off between safety, speed, and visibility?

BTW, for more experienced users, the default values can be changed via the setupsheets. You can make the default guess be anything you like or any expression.
jack9603301
Posts: 21
Joined: Tue Oct 12, 2021 6:10 pm

Re: About the diameter of the tool and the amount of cutting

Post by jack9603301 »

I agree with you, I think it is necessary at least to have a clear warning in the documentation, if possible, is it possible to make the guess more conservative and output a warning message when generating the toolpath?
Jipe
Posts: 35
Joined: Fri Apr 08, 2022 4:45 pm
Location: Narbonne France

Re: About the diameter of the tool and the amount of cutting

Post by Jipe »

Hi there,
Just the opinion of a recent FreeCAD user with a little experience in professional CNC machining. FreeCAD provides us with the essentials: the design and machining paths determined from tools selected from a database.
From these choices a tool path is generated taking into account the tool radius offsets (G41 or G42).

At this point FreeCAD has done the job; thanks to the developers. The choice of cutting parameters (cutting speed, feed per tooth, depth of cut, lubrication, etc.) is the responsibility of the user who, alone, knows the material on which he must intervene and the possibilities of his machine. (rigidity, spindle power, clamping technique...)

Unless you integrate a cutting parameters calculator in FreeCAD, I think the simplest solution for the user is to create a spreadsheet that allows in a few clicks to select a material and a type of milling cutter and instantly get spindle speed, feed and depth of cut settings. Some cutting tool manufacturers publish such charts, which apart from a few adjustments, allow you to start machining with complete peace of mind.

As @sliptonic pointed out, the best software in the world can't do it all, it requires a minimum of user investment to master the basics of traditional machining which still applies no matter what. , to the vast majority of CNCs.
jack9603301
Posts: 21
Joined: Tue Oct 12, 2021 6:10 pm

Re: About the diameter of the tool and the amount of cutting

Post by jack9603301 »

Unless you integrate a cutting parameters calculator in FreeCAD, I think the simplest solution for the user is to create a spreadsheet that allows in a few clicks to select a material and a type of milling cutter and instantly get spindle speed, feed and depth of cut settings. Some cutting tool manufacturers publish such charts, which apart from a few adjustments, allow you to start machining with complete peace of mind.
It might be more convenient to have a handy calculator, and as for the table, if it's optional, I think it's fine.

These are auxiliary tools in actual CAM programming. The actual parameter selection can only be guided by the user's own experience and the basic principles and knowledge of traditional machining, and there is no real general parameter.

Anyway, thanks to the FreeCAD developers.
Post Reply