Multi-axis ipm to dpm question

[Greg_J]

Hello,

I'm having issues with code that's being generated for a 4 axis tool path.

 

I have a round part that is chucked in our rotary axis and it has a flange protruding out of the side of it.

 

The stock for the part is round and was turned with material for the flange is round as well but offset.

 

I use a multi-axis program, parallel cut to "rotary rough" the part using the stock model. It keeps the tool cutting the material at all times and it is way more efficient then pocket roughing on many different planes.

 

During the roughing process the flange has flats on it as well as radii so during the cut the program moves from cutting the flat with out rotary axis movement then into cutting the radius while moving the rotary axis. The program moves back and forth from inches per minute to degrees per minute.

 

At times the rotary movement moves at a crawl and at others it move at a proper movement for the tool. I talked to Inhouse about this and the formula that is used in the post is correct and the feed rate is correct but when your running the tool it's obvious that the feed is incorrect.

 

So what results do you guys get when you make programs like this?

 

 

TIA,

Greg

[gcode]

do you have this turned on in your post

 

rot_feed : 0 #Use calculated rotary feed values, (0 = no, 1 = yes)

[Greg_J]

I'll have to check tomorrow and let you know.

 

Should all posts have that in them?

 

I have Fanuc and xxxxor posts that I'm working with.

[gcode]

I use InHouse mpmaster for 4axis work and that line is one switch it has.

The trouble with using degrees/minute is that the same federate will give

drastically different results on different sized part.

That's what that switch is for.. to tell the post to calculate the degrees/minute at the tip of the tool.

[Greg_J]

I seem to get feed that are correct for the tool then in the it will change the feed to a very slow dpm for a few inches of a certain move then it will go back to the correct feed. Using depth cuts it does this over and over again.

[Maclaw]

Hi Greg,

 

Go to:

 

Settings -> Control Definition Manager -> Find "FEEDS" in tree and enter it. At the "Rotary" section choose "unit/min" instead of "deg/min". You can also use "inverse feed" (it's the best choice). Anyway... Your problem should disappear. Save your Control definition.

 

Good luck!

[Nils N]

Maclaw, can you have "unit/min" and "inverse feed" both checked?

[crazy^millman]

13 days later glad you finally chimed in.

[Guest]

Maclaw, can you have "unit/min" and "inverse feed" both checked?

Can you have IPR and IPM checked at the same time?

[Maclaw]

Nope - it's a radio button - only one choice possible.

 

But You can use "unit/min" for the linear movement and "inverse feed" for the rotary movement under the "4 axis feed options" (and "5-axis feed options"). It works like this (assume you have unit/min for linear and inverse feed for rotary):

 

When there is no rotary movement in the block (no "A", "B" or "C" address) - the post outputs a G94 code ("unit/min") - the value after "F" is in IPM or mm/min. When there is rotary movement within the block, the post outputs a G93 code, which means the machine tool uses inverse feed under every F command. Both functions are modal. This is how it works under FANUC/HAAS posts.

 

I haven't seen IPR (Inch Per Round) option in the control def - not for for milling. It propably exists for turning. At least it's what I would suspect - but are not 100% sure.

 

Hope it helped...

[Maclaw]

13 days later glad you finally chimed in.

 

Yeah... well... better later than never... Maybe it's not obsolete yet.... :-)

[Guest]

Nope - it's a radio button - only one choice possible.

 

I was being sarcastic when I asked the question.

 

Linear moves will always be units per minute, rotary motion can be DPM or it can be Inverse from the Control Def's perspective. Reality is, if you're using TCPC you program in UPM and the control makes the calcs with no Inverse Feed needed.

[Maclaw]

 

Yeah Foghorn... I had that thought in the back of my head writing the reply.... But on the other hand I thought... what the hell! :-) Hey! I'm a newbie after all...