Missing G2/G3

[Bob K]

Good morning.

I'm having a problem this morning with my post not putting a G2 or G3 on a particular line.

 

N118 G3 X6.662 Z-6.5234 I.8634 K10.9967

N119 G1 X6.7086 Y-3.4653 Z-6.5255

N120 X6.7563 Y-3.5285 Z-6.5256

N121 X6.8057 Y-3.6216 Z-6.5198

N122 X6.8254 Y-3.6653 Z-6.5152

N123 X6.9152 Y-3.7021 Z-6.5169

N124 X6.9611 Y-3.7261 Z-6.5166

N125 X6.9608 Y-3.727

N126 X6.9573 Y-3.7407 Z-6.5136

N127 X7.2002 Y-3.7021 Z-6.5389

N128 X7.2005 Y-3.5189 Z-6.5677

N129 X7.2006 Y-3.4167 Z-6.5783

N130 X7.1917 Y-3.4098 Z-6.5782

N131 X6.6217 Y-3.4097 Z-6.5193 J.0138 I1.0056 K12.5268

N132 X6.6201 Y-3.4113 Z-6.519

 

Line N131 should have a G2 or G3. I see that the Y axis is only moving .0001. Not sure if that has anyting to do with the missing G code.

My machining center is looking for a "valid interpolation mode" to use with the I word.

 

Using V9.1.

 

Thanks,

Bob K.

[Trevor Bailey]

You may want to take a closer look at that line. I don't know of any control out there that outputs a G2 or G3 move in X, Y, & Z at the same time. You may have another issue going on there. What plane are you trying to machine in? What toolpath are you using, etc...

[chris m]

quote:

---

I don't know of any control out there that outputs a G2 or G3 move in X, Y, & Z at the same time

---

I think it would need to, Trevor, for any helical milling?

 

Bob K

 

What machine, control, and post are we talking here?

 

I think the missing code might be related to arc tolerancing; though I can't understand why it posted I, J, K but not the interpolation code?

 

[ 05-05-2003, 09:43 AM: Message edited by: chris m ]

[Bob K]

Hi fellas.

Shallow toolpath, using a modified MPFAN post.

Cincinnati machine with a Siemens Acramatic 2100 control.

I'm thinking tolerancing also.

 

Bob K.

[Trevor Bailey]

You are correct about the helical move Chris, except for one thing. Look at the first line where there is a G3 listed. It only has a X - Z - I - K segments in it. None of my posts have ever, that I remember, post all axis in a helical move.

 

Also, he is using a surfacing toolpath, not a helical.

 

He may have other issues.

 

[ 05-05-2003, 11:27 AM: Message edited by: Trevor Bailey ]

[McRae]

Variables drop only when 1/4, 1/2, 3/4 or full circles are interped. All positions may be required for incomplete or oblique interpolations. I have seen all 3 as well as the i,j values. The key is in the I,J,K values - a helix move will be perpendicular to the interp plane (G17,18,19) and so the corresponding I,J,K will drop out, not the X,Y,or Z.

 

Since this is a surfacing tool path, there is something wrong with the point as output from the NCI File - There isn't a G2/G3 missing, there is a problem with what the move type is in the toolpath generation. The post will only do what it is told to do - so look further up the data stream for the error. With the surfacing path - maybe it slipped into Multax somehow and the post doesn't support the rotary axes needed. For a 3ax path all the i,j,k's should be set at the start and that is it - all others to be ignored.

 

[ 05-05-2003, 11:37 AM: Message edited by: Andrew McRae ]

[Trevor Bailey]

Great explaination Andrew.

 

Bob, why don't you try the MPMASTER post from this site. It supports helical moves that your control uses. See if you get the same code from both posts and post back here so that we can also see, please.

[Nominal]

quote:

---

and so the corresponding I,J,K will drop out, not the X,Y,or Z.

 

---

Believe it or not some controls use the third vector component as the pitch of one complete rev of the arc in a helical interpolation. Not that this has anything to do with this guys problem. Just thought I'd mention it for accuracy.

[Trevor Bailey]

I have heard of a control that will be able to read/create arc toolpaths' say at a 45 degree surfacing toolpath. I can't remember which it was though.

[Allan]

quote:

---

I have heard of a control that will be able to read/create arc toolpaths' say at a 45 degree surfacing toolpath. I can't remember which it was though.

---

Sounds like a Siemans Control, the trick here is that the plane needs to be defined in the code before the arc.

 

 

Here is a blurb from Northwood Designs the makers of MetaCut Finish

quote:

---

Arcs may be fit in one of three methods: 1) relative to the standard orthogonal planes (XY,XZ,YZ). 2) relative to any rotation of the standard orthogonal plane. 3) to completely arbitrary planes (3D arcs). Almost all controls will machine arcs using the first method, some controls will allow method number 2, and a few controls are able to machined true 3D arcs. (*note- a 3D arc is not a helix).

---

HTH

[Bob K]

Thanks for the replies.

I downloaded the MPMASTER with the following result:

 

N121 G03 X6.662 Z-5.5234 I.8634 K10.9967

N122 G01 X6.7086 Y-3.4653 Z-5.5255

N123 X6.7563 Y-3.5285 Z-5.5256

N124 X6.8057 Y-3.6216 Z-5.5198

N125 X6.8254 Y-3.6653 Z-5.5152

N126 X6.9152 Y-3.7021 Z-5.5169

N127 X6.9611 Y-3.7261 Z-5.5166

N128 X6.9608 Y-3.727

N129 X6.9573 Y-3.7407 Z-5.5136

N130 X7.2002 Y-3.7021 Z-5.5389

N131 X7.2005 Y-3.5189 Z-5.5677

N132 X7.2006 Y-3.4167 Z-5.5783

N133 X7.1917 Y-3.4098 Z-5.5782

N134 G03 X6.6217 Y-3.4097 Z-5.5193 I1.0056 K12.5268

N135 G01 X6.6201 Y-3.4113 Z-5.519

 

The code is identical with the exception of the interpolation codes being put in their proper spots.

Before I posted this problem here this morning I put a G3 in the code at the control and the machine read right through it.

 

So where do I go from here? Looks like an issue with my post. Not sure where to look for the problem/solution in the post though.

 

Thanks again all.

 

Bob K.

[Joel Schreiner]

Bob

Did you try the mpmaster_A2100.pst.I know it works for the contour toolpath. Not to sure if it works for shallow toolpath. Also look at the post to make sure the switches are turned on to support a2100 helical milling.I hope this helps

joel

[McRae]

Bob K

 

 

This Morning

quote:

---

N131 X6.6217 Y-3.4097 Z-6.5193 J.0138 I1.0056 K12.5268

---

MPMASTER

quote:

---

N134 G03 X6.6217 Y-3.4097 Z-5.5193 I1.0056 K12.5268

---

Notice the difference now? There is a J value in the code and the z-ponstions are different. Sure MPMASTER puts in the proper code and you are working in the XZ plane for the interpolations so just what is it you wnat to accomplish with this move. Look furhter into the tool plane when you are generating the tool path and disable that nasty arcfilter - its not doing you anygood anyway.

 

Are you trying to use HighSpeed loops to connect?

 

[ 05-05-2003, 02:30 PM: Message edited by: Andrew McRae ]

[Bob K]

Andrew,

My bad. Should have looked closer.

So why did my post output the J, but not a G3?

The difference in Z value is part of the customization(sp) of my post.

I do have the arc filter on with a "total tolerance" of .003. You say this is doing me no good? Please explain.

Not doing highspeed loops intentionally. I'm using "follow surfaces" as my gap setting. Am I overlooking the highspeed settings with this toolpath?

 

Bob K.

[Trevor Bailey]

Try using the "one way" filtering. Did you update your post for the current version of MC that you are now running? Did you "tweak" your post yourself? What is your machining angle for the toolpath you are using? Are you using the "collapse" option made to overide resolution in accordance with the 3d cut method? There are many different options here. If your post has not let you down before, cut some air or a peice of wood to test the toolpath.

 

Personally, I would use the latest MPMASTER post from this site.

[gcode]

An email went out last week about V9.1 and posts.

It said to be sure the variable "arccheck" was set to 1.

See the Patches link above for details.

[McRae]

quote:

---

I do have the arc filter on with a "total tolerance" of .003. You say this is doing me no good? Please explain.

---

If you filter an arc that is only .003 in length, then you are only consolodating 3 linear moves anyway. Looks like the file is being drip fed so there is no real imputus for making the code smaller. This is my opinion/preference so do what you need to and are comfortable with. Also look at the magnitude of the K value - a 12" radius on a move that is only .050" in length might as well just be straight!

 

I was thinking of the roughing paths where you can use the loop connect on ends of the tool path. Looking into the surface finsih shallow parameters just now, looking quickly, I have no advise on what to do to eliminate the code or fix the error. Look further into the screen/configure options and change something and post until you get what you want.

 

quote:

---

So why did my post output the J, but not a G3?

---

If I could answer that then I would be able to sleep better this evening. Have you edited the post in anyway or is it just as shipped? With G-Codes post above, I would look into this as well.

 

Short on answers but hope we are steering in the right directions.

 

[ 05-05-2003, 03:39 PM: Message edited by: Andrew McRae ]

[Bob K]

Trevor,

Yes I'm using the one way filtering.

My post was a paid mod. and is updated to V9.1.

Angle is set to 45 and I'm not using the collapse option. Should I be?

Maybe I'll have to look into having the current MPMASTER modified for our use.

 

gcode,

I received the email and checked for the arccheck variable. Problem is my post doesn't have that variable. Could that be part of the problem here?

 

Andrew,

No drip feed here. So reducing file size does help somewhat. Our biggest gain with using the filter is surface finish. I do agree that this particular instance may not be the best candidate for it though.

I will look further into the screen/config settings.

Have a good evening and get plenty of sleep.

 

Thanks,

Bob K.