5 AXIS VECTOR RETRACT

[haroldm]

Hi all, i have jumped on the 5 axis toolpath bandwagon for the first time and i am trying to figure out a few things. Quick setup: we recently bought a Tr-Tech 5 axis head attachment for our Haas, and it came with its own Post processor, specifically the M5400Post. I can and will call them for this technical issue, but they are not open yet in California, so i thought i would turn to the forums in case someone else has ever experienced this. My problem is like this. When ever i finish a toolpath, and say the tool is done at a 45 deg angle, the post processor wants to put in a G49Z0 command and that basically removes all information about the tool and sends the tool back to zero wich could ruin my part depending on the angle that the cutter was left at. Now i have never programed a 5 axis before, so i was wondering, is it neccessary to put in say a 3d geometry point that acts like a lead in and lead out, or is the post supposed to handle this for you? The mastercam post is fine, but the machine requires we process the NCI thru their processor and that is what adds these issues, not mastercam. anyways, thank you for the help.

[Ployd]

We don't set up any geometry but we do use the clearance set to absolute which is based off of the geometry you are cutting. I usually set clearance to 2".

[Steve Hattori]

Harold, if you are using the Adv Multi-axis, you can set it in the link params to retract in the tool axis to the clearance Ployd refered to. That pulls the tool clear of the part so G49 doesn't crash it...

[haroldm]

hey guys, thanks for the response, let me look into it, thank you!

[haroldm]

hey Ployd, if i am using advanced axis control, where is the clearance set? When i use the regular 5 axis swarf (non advanced), all of my values are set to incremental, absolute is turned off, i dont get the option. and is the link you are referring to the "last exit 'back to clearance area'"? Thanks again

[JohnW@Kauffman]

I think Ployd is referring to the Clearance button at the bottom left on the link tab page.

[haroldm]

thanks john, i will try that.

[haroldm]

hey john, one question: i have used the clearance tab and that seems to be what i am looking for, but out of all the options, i cant seem to get the tool to retract at the exact same angle over a said distance, for example, the tool is stopped at a 52 degree angle, how can i make it retract at the same angle over a predetermined distance? Is the key in the exit macro options? Thank you

[crazy^millman]

Harold look to the point toolpath. Set a point in the same cplane to a place you want to clear. Then use the point toolpath on that same C-plane and it will bring the tool up after or before an operation with the correct angle and place so you know you are getting exactly what you are looking for and not some linking or clearance options from an operation that may or may not clear the part the way you want.

 

HTH

[Guest CNC Apps Guy 1]

On Head/Head style machines I ALWAYS use Point Toolpaths to direct positioning and retracts. MUCH safer that way.

 

JM2C

[JohnW@Kauffman]

+1 to the point toolpath. I have used these to position the tool safely on several occasions. I trim parts that sometimes have unusual shapes/curves and on a few parts I've created geometry and used the 5 axis curve with axis control lines as a transitional toolpath to move the tool exactly the way I want it. That's probably not the most efficient way, but it works for me.

[haroldm]

hey guys, specifically i suppose CNC_Apps, our default machine definition is set for Head_table..should i change this? I am not sure what head-head is? And as far as using points, so if i was doing a swarf toolpath, much like directing the entry for a pocket toolpath, lets say i could just creat a point and choose that geometry first?

[Guest CNC Apps Guy 1]

You should really only change the machine def if you're not getting the correct output. But personally, I like my machine def to to match my actual machine for example on an HMC X an Y are on the column and Z and B are on the table in reality, but on a typical MD in Mastercam it's not setup that way. Both give good code, but one accurately represents the ctual mchine ituation and one does not.

 

If your pocket is on a side/front/back face you'll want to pick the point in the top t/c plane to get it into position, then change your t/c plane to the face of the feature, then select the same point than do your toolpath and do the reverse point selection as you did initially. Not absolutey efficient as far as machine motion and only costs you a few seconds, but safe which is the most important IMHO.

 

 

Oh, Head/Head means that you have two rotary axes on the head.

 

HTH

[crazy^millman]

quote:

---

on a few parts I've created geometry and used the 5 axis curve with axis control lines as a transitional toolpath to move the tool exactly the way I want it.

---

The best way I know off!!!!!!!!!!!!

[haroldm]

Thank you all for your help, i believe i got a handle (of sorts) on the issue.

[Jim at Gentex]

quote:

---

i cant seem to get the tool to retract at the exact same angle over a said distance, for example, the tool is stopped at a 52 degree angle, how can i make it retract at the same angle over a predetermined distance?

---

This sounds like you want a plane retract move.

For a Heidenhain control, G174 is a full plane retract.

I'm not sure about Haas.

If you can find the right gcode for a plane retract you can put that right in your post.

 

HTH