Hello Guest it is October 15, 2019, 03:05:01 AM

Author Topic: NFS Turn Wizard  (Read 227810 times)

0 Members and 2 Guests are viewing this topic.

Re: NFS Turn Wizard
« Reply #50 on: November 21, 2011, 07:40:54 AM »
OK, I agree, stock size as Xstart makes sense. It is the starting X value, and the wizard will make its first cut at Xstart- cut depth.

Ill get a new version out with that and a few other fixes soon.

EDIT!

In the current version I calculate an actual cut value that is less than the one specified, but will make an integer number of cuts. In my new code I  make the cuts as requested, and the last cut may be some small value. Is this better?

I just realized that the Face operation does the same thing-- it makes its first cut at the Zstart value. Is this OK? or should I also assume Zstart means the end of the stock before the face operation.

On another topic, Id like to add a filet at the end of the turn operation. That seems like a common need. But I dont understand how to specify the G03 move. If I use I,J mode how do I deal with Dia vs, Radius/ Anyone understand filets in turn?
« Last Edit: November 21, 2011, 04:53:09 PM by Ron Ginger »
Re: NFS Turn Wizard
« Reply #51 on: November 22, 2011, 01:03:44 AM »
In the current version I calculate an actual cut value that is less than the one specified, but will make an integer number of cuts. In my new code I  make the cuts as requested, and the last cut may be some small value. Is this better?

I think the first way is better. Unless they enter the depth correct you will need to calculate actual cut depth anyway. I would prefer it respect my finish pass depth. This way you could control chip load for consistent
finishes.

Also any CAD/CAM or conversational control, the depth of cut is maximum depth not actual.
 
I just realized that the Face operation does the same thing-- it makes its first cut at the Zstart value. Is this OK? or should I also assume Zstart means the end of the stock before the face operation.

My vote is for z start to be end of stock.

On another topic, Id like to add a filet at the end of the turn operation. That seems like a common need. But I dont understand how to specify the G03 move. If I use I,J mode how do I deal with Dia vs, Radius/ Anyone understand filets in turn?

I no longer have access to a lathe cad system, so maybe someone else could do this.

   Draw and program a simple shape with radius on end.
   Send you a print of what was programed.
   Send you the g-code output by CAM system.

I am in the process of getting parts to convert my Okuma LB15 to Mach. These wizards are exactly what I was looking for.
Thank you for making these Ron

Mike

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: NFS Turn Wizard
« Reply #52 on: November 22, 2011, 07:34:06 AM »
The two Cams I have used (FeatureCAM and Dolphin) I think  keep the DOC at the setting you put per pass and if needed the last pass will be less. Then you do a finish pass as a second operation.

Fillet on a turning op would hopefully be optional?

Agree Z Start should be end of stock and all cuts are that less DOC.

FeatureCAM put in R's and Dolphin, which I use now, uses IK,  not sure how it does things but I think it will be in the Post Processor that the way things are done is defined. I know there are Rad and Dia posts for Dolphin, will have a look and see if I can work it out.
Hood
Re: NFS Turn Wizard
« Reply #53 on: November 22, 2011, 09:10:46 AM »
On the depth of cut I guess I cant win- some like it each way. I had some complaints on the Mill wizards about not following the requested cut. Ill see how ugly it would be to add a check button for user choice.

Face will be fixed to assume Zend means end of stock and first cut will be off that. Same issue here as in turn as to even cuts or follow the entered number. Again, if its not to ugly in the code ill offer a choice.

Radius could be set to zero to get a sharp corner- at least as sharp as your tool.

I got out my Smid book and have been reading about turn and radius. Since this is so common you would think Id find an example, but I will keep digging.

Thanks for the inputs.

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: NFS Turn Wizard
« Reply #54 on: November 22, 2011, 02:16:59 PM »
I think most facing operations are really just done to clean up the stock face so the majority would be done in a single pass anyway.
Still not had a chance to compare the Posts but will try in a bit.
Hood

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: NFS Turn Wizard
« Reply #55 on: November 22, 2011, 04:09:28 PM »
Ron, just looked at the posts and here is the only thing I can see that would relate to G2/G3 for Dia and Rad
Rad post is
#I = { $XCEN:XARC }
#K = { $YCEN:YARC }

Dia post is
#I = { $XCEN:XARC }
#K = { ($YCEN/2):YARC }

In the Dolphin Posts for Turn X axis is Z and Y axis is X ;D

Hood

Offline RICH

*
  • *
  •  7,367 7,367
    • View Profile
Re: NFS Turn Wizard
« Reply #56 on: November 22, 2011, 07:28:08 PM »
Ron,
If you want turning example codes have a look at Mach3 Turn - ARC Motion in Members Docs ( page 13 to 19).
I believe i posted the code for all the examples so you can actualy run the files  and see the affects of the differences using the G02 & G03 commands on the lathe.
Covers a lot of territory .......

Hopefully I will get some time and test out the wizard this weekend. You need to realize that everyone will appoach turning somewhat differently.


Hood,
Are you using the available Mach post processors for Dolphin?

RICH

Offline Hood

*
  •  25,855 25,855
  • Carnoustie, Scotland
    • View Profile
Re: NFS Turn Wizard
« Reply #57 on: November 23, 2011, 05:52:40 AM »
Rich,
 I modified the standard Dia post quite a bit to suit my lathe and what I wanted. Things I did were

                Toolchange position is for turret in use and not turret that is next.
                Threading changed to G76 rather than G32
                Coolant is dependant on tool used
                M5 will be issued befor M3/M4  if spindle is to be reversed
                Modality  has been changed so that code is only written if position will change
                Arcs are reversed if front turret iin use
                X values negated if front turret in use
                Drill cycles now produced long hand rather than canned cycles
                G90.1 inserted in preamble
                Changed threading Rules for both External and Internal to produce correct thread  height from nominal and pitch dimensions.



Hood
Re: NFS Turn Wizard
« Reply #58 on: December 05, 2011, 04:10:17 PM »
Brand new user here and a bit clueless. Sorry if these questions have already been covered but I didn't find the answer.
1. Where is the Single Step button in NFS Wizard?
2. I wish I could set the Plunge Rate (z axis) independently from the z axis. Any way this can be done?
3. For the same jog speed, the tool behaves very differently in x and z directions. This is probably due to very different screws. I'm I condemned to change the jog speed when going from one axis to the other or there is a way around this problem, how do you guys do?

Thanks,
Gaston

Re: NFS Turn Wizard
« Reply #59 on: December 06, 2011, 07:56:30 AM »
1)I tried to keep the screen simple so I didn't put all the jog controls on the main screen, but the TAB key pops up a full jog window, just like the main mach screen. Or do you mean the single block setting for running programs?

2)I don't understand this. What plunge rate do you mean, on the drill screen?

3)I have never heard of that being a problem. I don't think its possible to have different jog rate. You could use motor tuning to slow the faster axis, but then all your G0 moves would be slower.