1. расфрезеровать колодец под коническую резьбу
2 , нарезать резьбу резьбофрезой
1. отверстие отфрезеровано с применением фичера "фрезерование по линиям рез а ".
Если фреза берется с радиусом при вершине, обработка рвется. Лучше выбрать концевую. Тоже не супер, но СДЕЛАНО.
2. а вот собственно "резьбофрезерование» - Большая Головная боль! Получаем перемещение по 3 координатам без отработки коррекции на радиус инструмента.
Вопрос: как сделать, чтобы отрабатывались G41, G42
1. фрезерные отверстия конической резьбы
2 резьбовые Резьбофрезерование
Нет дополнительных линий
big headache: no additional lines
tool radius compensation not working
that tool path looks like it is for a single form threading tool which I have not tried with Creo3.0 . I believe that cutter compensation will not work with a helical toolpath. You would have to compensate with the tool diameter to adjust the thread diameter.
Sorry I have not responed to you before this but I can't seem to translate your questions.
CREO3 milling component conical surface along a helical - additional turns of are not created!
" I believe that cutter compensation will not work with a helical toolpath. You would have to compensate with the tool diameter to adjust the thread diameter."
compensate with the tool diameter to adjust - Trying to say that does not work!
sorry for my english
With a rough translation it sounds to me that you are trying to do a tapered thread but cannot get radius comp to turn on. First question, does your tool have multiple teeth on it? Meaning you can do the whole thread depth with one pass? I see in one of your screen shots that you have a toolpath with several passes to get your thread depth. If your tool only has one row of cutting teeth on it I am not aware of Creo being able to do a “thread mill” sequence for a tapered thread. In this case you will have to set up a helical mill profile and it won’t be near as easy. I am only on Creo 2 so maybe this is new to Creo 3. If you do have a tool that will complete the thread in one pass try this:
In your tool setup make sure you have a value for tool insert and number of flutes(this is actually number of rows of cutting teeth) This is how I have this one set up (remember I’m using inches)
Then in you thread milling sequence you will need to set these parameters. LEAD_RADIUS, TANGENT_LEAD_STEP, NORMAL_LEAD_STEP, APPROACH_TYPE, EXIT_TYPE, ENTY_ANGLE, EXIT_ANGLE, CUTCOM. I am doing an M14 x 1.5 thread with a .4 dia tool:
I like to have a tool path that starts in the center of the hole, turns dia comp on with a straight move, ramps into the cut, makes one complete circle, ramps out of the cut, does a straight move back to center turning dia comp off. I calculate LEAD_RADIUS and TANGENT_LEAD_STEP by taking this formula: “major dia – tool dia X .2” NORMAL_LEAD_STEP will always be 0. APPROACH_TYPE and EXIT_TYPE are HELICAL. ENTRY_ANGLE and EXIT_ANGLE are 140. And ENTER and EXIT from AXIS are YES. And of course CUTCOM must be ON. Here are a couple views of what this looks like:
And here is the CL Data:
number of flutes(this is actually number of rows of cutting teeth)
In this case you will have to set up a helical mill profile and it won’t be near as easy
I will do - will write