When I go to settings and then select 8’’ 4th axis , all I find is directions to tram it in . What I am looking for is a place where I can fill in the blanks where I can get a program to generate a thread like form . I cannot find any that shows me how to use the A axis and X axis in conjuction to get the result that I want . Why does’nt Pathpilot have this in the conversational section ?
Thanks in advance ,
ErnieD
Ernest,
Pathpilot doesn’t have any conversational functionality that incorporates use of a 4th axis, there are a lot of features such as this that we could develop but development time is limited so priority must be given to features with the greatest impact to our entire userbase.
I wouldn’t think that such a design is too complicated to program by hand if you can have a tool that matches the profile, but otherwise you would need to use a CAM package for programming.
Thank you,
Norman
What I am looking for is what is the A function calling and what is the F function calling for . The X function is obvious . In A is it feed, rotation or something else . Is there anywhere in your data base where I can find this infro ?
Thanks ,
Ernie
Ernie,
“A” is calling out that the A axis should move to a given position, and since the A axis is a rotational axis it is in degrees. You will always need a position specified after the “A” or an error will be given.
“F” is specifying the feed rate to move at. It will either be specified in inches/millimeters per minute, inches/millimeters per revolution, or inverse time mode based on the feed rate control mode specified. Inverse time mode commands movement to be done in a given amount of time, this is the typical feed rate mode for coordinated linear/rotational axes moves. You don’t always need an “F” callout on every line unless you are using inverse time mode, the machine will apply the last specified feed rate.
The programming chapter of any of our mill manuals covers functionality of M and G codes.
Thank you,
Norman
Norman ,
I mean no disrespect but I believe the manual was written for someone that does not need a manual . I am 91 years old and the info that you gave me really meant nothing .
I think that I am going to go search some of the forums that are available and see if I can get an example of what I want to do ,
Best Regards ,
Ernie
No disrespect intended here either Ernest, just trying to figure out where you are in terms of program reading and writing. I can throw together a sample program for you but I need to know where you are in terms of knowledge so my response is more helpful.
I assume you have created programs using the conversational interface and so you understand things like setting your WCS, tool length offsets, etc. If not, please correct me. Have you ever manually written or edited a program once it’s been generated?
Are you looking for one specific thread or do you have a need for multiple thread sizes? What are you using for a cutting tool to make the threads? What material are you cutting?
Here is what I was looking for X-1.5 A3060 F .145 . The number in A = 360 x 8.5 (the number of revolutions) and the number is the lead or pitch .
In that case, the value in A is simply the number of rotations which in this context would be the total number of threads. It doesn’t represent anything about the pitch without taking the X value into account. To get that you need the following calculation:
Threads per inch = rotations/travel distance = (A/360)/X = approx 5.6667 tpi
Pitch = travel distance/rotations = X/(A/360) = .1765"
If you work those calculations backwards you can get the appropriate values for X or A depending on your desired pitch or tpi. For example, if you want 1.5" of thread at 12 threads per inch:
12 = (A/360)/1.5 =>
12 * 1.5 = A/360 =>
12 * 1.5 * 360 = A =>
A=6480
Or, if you want a pitch of .1" for 14 threads:
.1 = X/(14) =>
.1 * 14 = X =>
X = 1.4
For this situation you also need to calculate A which is just number of threads * 360:
A = 14 * 360
A = 5040