tool path returns to origin many times

[steve123]

Doing the test is possible. Automatically switching to a drill motion is a bad idea. The geometry of an endmill is quite different from a drill bit. As is the output gcode.

I was not clear ... I was not intending to suggest switching to a drill motion. Rather, since the user selected to use the profile operation for these circles instead of a drill, the gcode generated would be a plunge and retract and omit the circular path.

If radius is zero, the hole is not profilable and should be skipped, possibly with a warning in the console

That seems reasonable as well. I suggest that the user might want to override this behaviour and use the end mill anyway.

[steve123]

Flagging the error or preferrably just ignoring that location is fine. Changing the operation type to drilling automatically seems like a really bad idea.

Apologies, I was not clear and did not intend to suggest changing the operation type. Rather, implement the motion of the profile operation as a plunge and retract and omit the circular path.

[sliptonic]

Flagging the error or preferrably just ignoring that location is fine. Changing the operation type to drilling automatically seems like a really bad idea.

Apologies, I was not clear and did not intend to suggest changing the operation type. Rather, implement the motion of the profile operation as a plunge and retract and omit the circular path.

I understand. That's still a bad idea. Not all endmills can plunge. Assuming they can is a bad assumption.

[mlampert]

I understand. That's still a bad idea. Not all endmills can plunge. Assuming they can is a bad assumption.

Look at that - and I thought that was the definition of an "endmill"

[GeneFC]

I buy only center-cutting endmills.

They still aren't very happy plunging.

Gene

[sliptonic]

I understand. That's still a bad idea. Not all endmills can plunge. Assuming they can is a bad assumption.

Look at that - and I thought that was the definition of an "endmill"

If we're being pedantic, you're somewhat correct. An "endmill" is a milling cutter that can cut axillary. It still may not have cutting edges all the way to the center so might not be able to plunge.

A cutter that can ONLY cut radially should just be called a "mill". But the term "endmill" is used generically for both.

[steve123]

If we're being pedantic, you're somewhat correct. An "endmill" is a milling cutter that can cut axillary. It still may not have cutting edges all the way to the center so might not be able to plunge.

A cutter that can ONLY cut radially should just be called a "mill". But the term "endmill" is used generically for both.

The current "process holes" and 'process circles" assumes that end mill can plunge into the work piece. I wonder if a tools ability to plunge should be added to the tool properties? That way, the profiler could inspect the plunge property and create the profile accordingly.

[sliptonic]

If we're being pedantic, you're somewhat correct. An "endmill" is a milling cutter that can cut axillary. It still may not have cutting edges all the way to the center so might not be able to plunge.

A cutter that can ONLY cut radially should just be called a "mill". But the term "endmill" is used generically for both.

The current "process holes" and 'process circles" assumes that end mill can plunge into the work piece. I wonder if a tools ability to plunge should be added to the tool properties? That way, the profiler could inspect the plunge property and create the profile accordingly.

The objective of a profile is to cut the path radially with the cutter. To do that, we have to get the cutter into position. So, yes, it does default to a plunge because you have to do something. It's assumed that if the cutter can't plunge, the user will add a ramp dressup to the operation.

However, If the hole is exactly the size of the cutter, there's no room to ramp. I still say that changing the assumption from radial to axial cutting is a bad idea. From a machining standpoint, I don't think it's a good idea either. Real machinists can correct me but I think the cutter may deflect and have runout so you'd get a hole either the wrong size or wrong position (or both).

That said, adding such an attribute to the tool is a good idea. If nothing else a safety check could run and display a warning and add a squawk to the PathSanity report. You want to tackle that? It's very much like what I did to prevent the spindle being turned on if the probe is loaded.

[steve123]

That said, adding such an attribute to the tool is a good idea. If nothing else a safety check could run and display a warning and add a squawk to the PathSanity report. You want to tackle that? It's very much like what I did to prevent the spindle being turned on if the probe is loaded.

I can probably handle that. I will have a look at what you did with the spindle. I won't be able to get to it right away but I'll put it on my todo.

[freman]

Code: Select all

That said, adding such an attribute to the tool is a good idea. If nothing else a safety check could run and display a warning and add a squawk to the PathSanity report. You want to tackle that? It's very much like what I did to prevent the spindle being turned on if the probe is loaded.

This is not a binary. There is not a standard size of the non cutting part, either in mm or as a %age of tool diam., so that probably also needs a dimension of how much non cutting radius there is at the centre of the tool.

Generally I don't think the software should attempt to hand-hold numpties who do not know how to use their own machines and tools.

If a machinist decides he wants to plunge a hole with an endmill ( possibly to avoid a tool change ) he will have to ensure he has a suitable tool to plunge. Even a ramp is not clean if you do not have a tool which cuts to the centre since the non cutting part is still getting stuffed into the stock. Cutting speed will be way off at centre too.

Drills are pointy for a reason but sometimes ugly compromises are made for speed or other playoffs. I have previously criticised FC refusing to cut slots with a mill == to slot width and refusing to mill holes. ( IIRC it was projected area==0 or some such failing to differentiate tool larger than slot from tool == slot ).

IMO , this should be allowed by the software even though it is not generally the "proper" way to cut a slot. IRL things often get done in non idea , not best practice ways for legitimate production reasons. The user should be allowed to mill a hole if he needs to. If he did not realise why we have drills as well as endmills , he will learn from experience when looking and the result.

It's very much like what I did to prevent the spindle being turned on if the probe is loaded.

Nice, that makes sense.