9.1 Constant Rotary Feed Post Question

[CAM-mando]

Is it possible to force a constant rotary feed rate ?

 

I want to generate code for a CNC that will be timed to a seperate HAAS indexer and just pick a feed rate based on the "worst case".

 

For a simple example ... using axis substitution on a one revolution non linear rotary cut I want to program the indexer as one step of 360° at a constant feed rate. I want mastercam to adjust the X axis feed rate as neccessary to follow the geometry.

 

Could one of the post Guru's point me in the right direction ?

[JG]

cammando,

first off, I know very little about posts, having said that it seems to me you need to know the velocity of the indexer (seconds per rev), next I think you would need to get MasterCam NOT to break the rotary motion into smaller moves, then I think some sort of formula could be developed to have the linear and rotary axis arrive at the same time.

 

thanks,

 

Jg

[crazy^millman]

Could you edit feeds at point? Not sure if what you are after is possbile. The post is trying to make the feed be correct to liner feed at the spefic point of the tool relative to the dia it is cutting at the time. I do axis sub alot and like the way I get a very close to what I want code. I have used 5th axis and 4th axis stuff to make code but really hate all the garabe code you get doing it that way. Here some snippet from something I am working on this week.

code:

---

T2M06(T2 |  1/2 FLAT ENDMILL)

M01

G00G90G54X0.Y-12.8B-57.349S1200M03T18

G43H2Z24.183/M8

Z10.283

G01Z10.183F10.

B-56.325F562.66

Y12.8F100.

B56.325F562.66

Y-12.8F100.

B-56.044F562.66

Y12.75F100.

B56.044F562.66

Y-12.75F100.

B-55.762F562.66

Y12.7F100.

B55.762F562.66

Y-12.7F100.

B-55.481F562.66

Y12.65F100.

B55.481F562.66

Y-12.65F100.

B-55.2F562.66

Y12.6F100.

B55.2F562.66

Y-12.6F100.

B-54.918F562.66

Y12.55F100.

B54.918F562.66

Y-12.55F100.

B-54.637F562.66

Y12.5F100.

B54.637F562.66

Y-12.5F100.

B-54.356F562.66

Y12.45F100.

B54.356F562.66

Y-12.45F100.

B-54.074F562.66

Y12.4F100.

B54.074F562.66

---

See how I get F562.66 at the B moves then I get F100. at the Y moves all done in the post. BTW it is a modified MPMASTER post.

 

HTH

[Slepydremr]

Cam,

Does your control not handle INV feed rates? I believe that if you can turn on the INV feedrate in the post then it will maintain a constant feed based on the tools position from the center of rotation.. IE the closer it gets to centerline the faster the rotary has to spin.. I haven't figured out how to get mcam to put out a different feed for each z depth any other way..

[JG]

I'm guessing it is a "M" code indexer where the angle is specified on a seperate control box, in a seperate program....

 

Jg

[Slepydremr]

Well if that's the case then I would have to agree with what you said above above calculating the rotaries speed.

 

Hope fully there is a way to asjust it so that you don't break alot of cutters.

 

The only one I used like that rotated so fast it would have been impossible to do.

[mcpgmr]

I don't think this is what your looking for but there are some usefull calculators here.--

 

http://i-logic.com/utilities/index.htm

[CAM-mando]

quote:

---

I'm guessing it is a "M" code indexer where the angle is specified on a seperate control box, in a seperate program....

---

Corect. Sorry if I wasn't clear before.

 

Normally Mastercam maintains and effective feedrate defined in parameters page. The X feed and A feed are adjusted to maintain the chosed effective feed.

 

With a seperate indexer controller this would mean programming a bunch of steps with varying feedrates.

 

One approach is to tie the indexer into the control and using custom macro B and RS232 have the CNC control actually control the indexer. This is not possible with the CNC in question.

 

Another possibility is a post that post twice. The first time generates the CNC code with Mcodes for indexing and then re-post and generate an indexer program. I am working on this but it is a longer term project for the feeble little CAMmando brain.

 

Since most of the simultaneous 4 axis stuff done on this machine is fairly straightforward, I can usually use a combination of mastercam and manual programming to get what I need.

 

Other jobs are just slight variations on a helix. For these I thoght if I could Fix the rotary feed and let the X axis feed float, it would be a simple solution. Recognizing that the effective feed rate will be at times inefficient depending on how close to a pure circular cut the program gets.

 

I plan on diving into this again this weekend.

 

Thanks

 

Hey Paul I still use your rag tag centerdrill chart.

[crazy^millman]

I use to have to program 4th axis like this years ago. I found that dwell is your best friend. I had dwells all over the place to make up for the time difference the 4th axis would need to start after the Mcode was called. I would then just play with those till I got the desired effect or toolpath I was looking for. It was a real pain in the arse but did the trick. I feel for you and to do 4th axis work that requires full 4th axis with an external 4th axis is just asking you to lose money. I wish you good luck but you have a fight on your hands. You could make a post up that only outputs A moves and have it hard coded to output a Mcode every time it indexes.

 

HTH

[CAM-mando]

Yeah Ron we are on the same page.

 

Most of the parts I have put on this machine are not too complex. I have actually had suprisingly good success with timing with a little careful math.

 

There is about a 100 milisecond delay or so after calling the Mfunction that releases control back to the CNC. Usualy I have only had to use the dwell trick with higher feed rates on plastics.