custom tool / programming question

[riverracer]

hi all,

i created a custom single point thread mill, profile drawn to size (rad 14mm) with the shank (rad 9.5mm), (think slot saw), called it undefined, picked custom file and set the dia at 28mm. saved to tool libary.
do the lengths and arbor dia size boxes come into play or are the sizes taken from the drawing?

then in thread mill toolpath (top right hand side) it says 28mm. if i use comp type set as 'computer', it will use this value.
i wish to use 'control', so i can fine tune the part thread size at the haas control, with the actual exact tool size (approx 27.83mm) in the offset page.
so do i keep the same sizes ie; 28mm or do i have to set the actual tool size in any of these settings?

part is approx 34mm dia, thread depth 1.5mm, giving minor dia of 31mm. this is what i have set in m/cam. then i will set the haas tool offset to say 28.2 dia, take a pass/passes, measure, decrease down to the exact tool size as needed. am i on the right track?

lastly, in backplot the tool shows up, but sometimes in verify on a solid, the tool dosent show, all that happens it the % counter counts up to 100% and thats all, no change to the solid.
is this a graphics setting or something i set wrong on the tool pages when i have been playing?

this is all in x4mu3
threads are for a mould, so only about 4 being made.


thanks

[Superman]

You are on the right track,
a custom tool drawing is drawn 1:1
....the tool drawing is NOT used in any form to calculate a toolpath
....no operation in mastercam uses your selected drawing to calculate a toolpath
...toolpath calculation is done using the sizes you have set for that tool

The drawing is for graphic use only in backplot and also in verify
In verify, Mcam uses the tool shape to remove pixels out of the stock to give a close approximation of the machined part

my comments in eMastercam


The threadmill operation can be done by selecting a point or a circle
...if by point, the operation's parameters holds the thread OD value you want to achieve
...if by a circle, there is no indication of what Ø you are doing unless you analyse the geometry

best to use a point, as you can drag & drop the spotting/drilling geometry into the next op and you know it is the same c'points for all

then in thread mill toolpath (top right hand side) it says 28mm. if i use comp type set as 'computer', it will use this value. i wish to use 'control', so i can fine tune the part thread size at the haas control, with the actual exact tool size (approx 27.83mm) in the offset page. so do i keep the same sizes ie; 28mm or do i have to set the actual tool size in any of these settings? part is approx 34mm dia, thread depth 1.5mm, giving minor dia of 31mm. this is what i have set in m/cam. then i will set the haas tool offset to say 28.2 dia, take a pass/passes, measure, decrease down to the exact tool size as needed. am i on the right track?

if you set to:-
- "Computer" - no capability of using offsets are output, adjust tool Ø in Mcam and re-post each time until you get it right
- "Control" - an offset in the control of 0 will make the tool run on top of the thread OD, a value of 28 would offset the cutter to finish the thread OD---typically, you dial in the tool Ø and it will give correct size
- "Wear" - the required shape is offset by the programmed tool radius, an offset in the control of 0 will make the tool run on this "offset" profile, inputting a -ive value makes the cutter cut more into the part, a +ive value would make the tool run further away from the thread OD ( you start with a small +ive value )

principle of using control comp
- tool rad set = 0 in the control, tool cuts on centreline, part is stuffed
- tool rad set = actual Ø in the control, part is finished to size
- tool rad set > actual Ø in the control, part has material ON
- tool rad set < actual Ø in the control, part is stuffed

principle of using wear comp
- tool rad set = 0 in the control, actual tool used is as programmed, part is finished "on size"
- tool rad set = 0 in the control, actual tool used is smaller than programmed, part has material ON ( tool needs to be comped in, a -ive value is required )
- tool rad set = 0 in the control, actual tool used is bigger than programmed, part is stuffed ( +ive value is required )

The toolpaths outputted are the tool centreline
you should not mix "Control" and "Wear" comps on the same tool in different Mcam operations

eg. a toolpath created for a 12mm and a 10mm cutter is used, comp value in the control should be -2
NOTE... "wear" sometimes can only take a small amount of adjustment, depending on the internal arc sizes on the toolpath


If you get an error when posting the threadmilling regarding "incorrect toolplanes" or something similar,-it may be that the lead in/outs clearance needs adjusting so comp starts & finishes with a line, also set start on hole centre point ...ON.

boy...my finger is sore...what an essay!!!!
getting cold down here n Mexico, what's it like up in banana land ??

[jonathanw]

Superman, I have a couple of questions that you may be able to answer. All of the custom tools that I have created have been lollipop endmills and I always have to scale the cutting diameter to 2.0 inches in order for them to display correctly. However I have seen a couple of your post and you state that it should be 1:1. Is this because of the type of tool being defined or maybe an earlier version of mastercam? I run X4.
I have also run into a problem when regenerating a toolpath using a custom lollipop, an error will come up stating that the shank and cutting diameter must be the same. So if I am using a .375 cutting diameter with a 0.5 shank, I have to change the shank to match. Then I can regenerate my toolpath. Just thought of this, I am so used to saving all my work on a thumb drive and that is where I keep my custom files, I suppose they should be saved in the tool folder correct?

Thanks Superman

[Superman]

All of the custom tools that I have created have been lollipop endmills and I always have to scale the cutting diameter to 2.0 inches in order for them to display correctly. However I have seen a couple of your post and you state that it should be 1:1. Is this because of the type of tool being defined or maybe an earlier version of mastercam?

Tools are done the way you are doing it, with the exception of Undefined tools, which are dawn 1:1

I have also run into a problem when regenerating a toolpath using a custom lollipop, an error will come up stating that the shank and cutting diameter must be the same. So if I am using a .375 cutting diameter with a 0.5 shank, I have to change the shank to match. Then I can regenerate my toolpath.

I think this is needed for the toolpath calcs,, like 5 axis port machining, or breaking edges on a back face in a hole
9 times out of 10, the shank is the same or larger than the tool diameter. There will be exceptions of course (ie a rotary burrs, or mounted grinding wheels/stones etc)

I assume you are applying the file to the lollipop icon and not a different tool icon.
The toolpath is calculated from the input values on the toollng page. and is never,never taken from the drawing file
The drawing is ONLY used for the graphical display in backplot and verify

Just thought of this, I am so used to saving all my work on a thumb drive and that is where I keep my custom files, I suppose they should be saved in the tool folder correct?

The toolling files should be accessible at all times, if they are not available when the file is opened, then the drawing you have attached to the tool is removed and the default shape is assumed (ie . you can have a threadmill drawing attached to a flat endmill ( so it verify's correctly ), but if that drawing is not there on opening, then the standard flet endmill MCX file is in its place)

[jonathanw]

Originally Posted by Superman Tools are done the way you are doing it, with the exception of Undefined tools, which are dawn 1:1

Good to know. I have been told to upscale every tool. Is there a certain reason why the standard tools have have be upscaled, but an undefined tool does not?

Originally Posted by Superman I think this is needed for the toolpath calcs,, like 5 axis port machining, or breaking edges on a back face in a hole 9 times out of 10, the shank is the same or larger than the tool diameter. There will be exceptions of course (ie a rotary burrs, or mounted grinding wheels/stones etc)

I suppose that would make sense since you are unable to define all the aspects of the lollipop, such as the taper. Would it be possible for the posted toolpath be different from the verified toolpath if I do define the shank as the same size as the cutting dia. but the toolpath verifies correctly?

Originally Posted by Superman I assume you are applying the file to the lollipop icon and not a different tool icon.

Yes I am applying them to the lollipop icon.

Thanks

[Superman]

Originally Posted by jonathanw I suppose that would make sense since you are unable to define all the aspects of the lollipop, such as the taper. Would it be possible for the posted toolpath be different from the verified toolpath if I do define the shank as the same size as the cutting dia. but the toolpath verifies correctly?

It is the tool drawing that gets used to take the pixels off the screen when verifying, that is why I used a thread mill drawing on a flat mill icon as an example....change it to a differnt tool shape drawing..ie dovemill, or even a drill

You really need the tool drawing to be as accurate as possible----you could add on part of the holder to highlight possible collisions ( shank/holder area about .01"-.02" accuracy tolerance )...but always draw to the max size it'll be...then you are on the safe side.

You then pay close attention to what the tool and shank and "holder" is doing on backplot and/or verify ...altering any part of the tool definition, to get into or stay away from a desired area, will force a regen....but you did draw the tool and holder accurately as to be able to catch any gouges...you can also "compare to STL" to highlight a stock ON or OFF condition