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
if you set to:-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?
- "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 ??