Help With dynamic milling

[floo]

Hi!

Im making a part and im using the optirough toolpath with coremill passes, but the thing is when the machine "retracts in X andY" to take the next cut, it doesnt go "outside" of the part, it goes where the previus cut has been made in X and Y,so its kinda scrapes the part on the way back, i know that you can set a microlift distance in Z, bur how for X and Y?

Sometimes it feels like it makes "shortcuts" around corners when roughing, can this be related?

Thanks

 

hope ive made my self understood?!

[dfedwards]

You can try increasing your toolpath radius or decrease your Gap size and set Motion > Gap size, retract drop down to use gap when avoiding a boundary OR exceeding a distance. This will cause a lot of vertical retracts but it is better than violating the part in back moves. I would like to see a setting to adjust the distance the tool stays off the material in back moves but I don't know of anything other than what I mentioned. Hope this helps, if anyone else know of anything else, I would like to know also.

[dfedwards]

I was curious to see someone elses input on this. Anyone else got input?

[Goldorak]

there is no dedicated parameter to set the clearance in optirough (hope for X6), i do like dfedwards , boost the radius or use "full retract" with a small gap

 

our older machines tend to chop the corners at high feedrate back move

[floo]

thank you for you answers, i will have a go at that!

Is there anyway possible to have all retracts as G0 instead if G1 with hight feed(it gets abit jerky with the changes of feeds all the time

[dfedwards]

thank you for you answers, i will have a go at that!

Is there anyway possible to have all retracts as G0 instead if G1 with hight feed(it gets abit jerky with the changes of feeds all the time

 

Sure, On the liking parameters page, You can set the retract dropdown at the right to "Full Vertical Retract" or use "Minimum Vertial Retract" and uncheck the Output feed move checkbox. A word of caution unchecking the output feed move checkbox, most machines do not do true vector rapid moves meaning that the x and y axis rapid at the same speed so your rapid move will not be a straight line and this could cause a collision on the machine that you will not see in Mastercam. Hope this makes sense, I know what I'm trying to say, not sure I communicated it effectively.

[floo]

ok, lets se if iget this right, if i want the "retract" in X and Y as a G0 instaed i just uncheck outout feed move checkbox? is that correct?

[dfedwards]

ok, lets se if iget this right, if i want the "retract" in X and Y as a G0 instaed i just uncheck outout feed move checkbox? is that correct?

 

I may be misunderstanding your question. You ARE talking about retracting above the part in Z first right? If so, then yes, it will retract in Z at rapid first, the reposition X and Y with a rapid move, the rapid back down in Z to feed plane as detrmined by settings in transitions page and linking parameters Leads, then feed into next cut.

[floo]

No, i mean in X and Y, sorry if i didnt make me clearm but i didbt find a better word then "retract", im from Sweden.

So what i mean is when i output i higher feedrate example 10000(metric) for a X Y position to take the next cut, i want that to be a G0 instead of G1

 

Hope you understand

[Guest CNC Apps Guy 1]

No, i mean in X and Y, sorry if i didnt make me clearm but i didbt find a better word then "retract", im from Sweden.

So what i mean is when i output i higher feedrate example 10000(metric) for a X Y position to take the next cut, i want that to be a G0 instead of G1

 

Hope you understand

 

You may think you want a G0, but you REALLY do not. Your machine motion will most likely become jerky, and as was stated, you could end up with dogleg traverses instead of linear montion. Danger Will Robinson!!!

[dfedwards]

Personally, Ii wouldn't want to rapid while the tool is down in the part. As I mentioned earlier, rapid moves typically are not vector moves so the path is not controllable as a straight line. I don't know of any way to make Mastercam do this either. Sorry I can't help with this one.

[floo]

ok, i will try to tweak the feeds, thank you for all the help