[CROSSHATCH]

Hello everyone,

I'm looking to solve this issue but I'm not sure there is an easy way, hopefully their is.

Previously, I did all my CAM inside Inventor (hsmexpress) and used the Post Process of Mach3. Here is a sample of my block and coding for tool changes that has worked great.

(1001)
(004 PROFILE CLEARANCE)
(T5 D=0.375 CR=0.015 - ZMIN=-0.8374 - BULLNOSE END MILL)
(T6 D=0.25 CR=0. TAPER=45DEG - ZMIN=-0.05 - CHAMFER MILL)
(T9 D=0.375 CR=0. TAPER=118DEG - ZMIN=-0.1 - CENTER DRILL)
(T26 D=0.135 CR=0. TAPER=135DEG - ZMIN=-0.8874 - DRILL)
G90 G94 G40 G49 G17
G20

(2D CONTOUR1)
M5
M9
T5 G43 H5 M6
S5000 M3
G54
M8
G0 X0.7975 Y6.0094
Z0.6
Z0.2
G1 Z0.1375 F35.
G19 G2 Y5.972 Z0.1 J-0.0375 K0. F50.
G1 Y1.6025 Z0.0811
G17 G3 X0.82 Y1.58 Z0.0809 I0.0225 J0.
G1 X0.855 Z0.0808

Other than the title and perhaps an interesting piece is the G43 of the Inventor Generic Mach3 post title. I switched all of Solidworks settings to match my good, verified, qualified G-code (as shown above). However, when I save the Solidworks post, with the same settings I have some extra codes that have shown issues.

Attachment 323840
Inventor

Attachment 323842
Solidworks

Here is the Solidworks code:

(0004-0001-WARMUP-2)
(WARM-UP TEST2)
(T4 D=0.5 CR=0. - ZMIN=-0.43 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G20

(2D ADAPTIVE5)
M5
M9
T4 M6
(ER32 COLLET)
S6000 M3
G54
M8
G0 X-0.3648 Y-5.2405
G43 Z0.6 H4
Z0.2
Z-0.33
G1 Z-0.38 F30.
X-0.3645 Y-5.2403 Z-0.3856
X-0.3637 Y-5.2399 Z-0.3911
X-0.3624 Y-5.2391 Z-0.3965
X-0.3605 Y-5.2381 Z-0.4017
X-0.3581 Y-5.2367 Z-0.4066
X-0.3553 Y-5.2351 Z-0.4112
X-0.3521 Y-5.2333 Z-0.4154




Where is the G91.1 code coming from? What am I missing? Also, this G43 Z0.0 H4 would have wreaked havoc if I was not test cutting air. From my pursuit, removing G91.1 and removing that entire line starting from G43 has shown that the code does not try to stop and travel upward in the Z-Axis. Typically (with Inventor post) it stops, I hit cycle start and the tool number changes. At this point I am free to move and make a toolchange and when ready; hit cycle start. This with the new loaded offset is set for the next cycle. But with G43 it was stopping and going up some distance, setting to Z0.0 and starting at this elevated plane.

What is adding this and how can I go about NOT having to edit the G-code for these lines or safety blocks? I am able to search through the code and delete what I need but it would be nice to be automated like when with Inventor.

Regards,

-Jason

[ger21]

Where is the G91.1 code coming from?

From your post processor.
G91.1 forces Mach3 to use Incremental IJ mode, which is a good think if Mach3 happens to be in absolute IJ mode when you load your g-code.

The bad thing, though, is that G91.1 can NOT be on the same line as a G90 or G91, or one or the other may not work. Most people are not aware of this, and many post processors do this.
I believe that all of your issues are caused by the post processor, but I don't use your software, so can't really help with it.

[SCzEngrgGroup]

The line of setup codes comes from the POST - it is generally hard-coded, so you need to edit the POST to change it. The G43 Z0.6 H4 should be harmless. It is just a single line that sets the tool length offset, and does a Z move to +0.6.

Which POST are you using?

Regards,
Ray L.

[kvom]

I have read that Mach3 does not handle G42/G43 correctly in all cases. YMMV.

[ger21]

G42 and G43 are two different things. G43 works fine, afaik.

[CROSSHATCH]

The Inventor post provides this line: "T5 G43 H5 M6" which has not caused any issues.

The Solidworks post puts G43 on a different line:

T4 M6
(ER32 COLLET)
S6000 M3
G54
M8
G0 X-0.3648 Y-5.2405
G43 Z0.6 H4


All I know is that my machine runs correctly with how the Post comes from Inventor but does not do so with the Solidworks post.



Ray- I attached both POSTS to show that I am using similar/same settings. Except, Soldiworks keeps inputting G91.1 and adding G43 to separate line which is causing my machine to not function accordingly.

Regards,

-Jason

[CROSSHATCH]

The Inventor post is named "Mach3mill-G43.cps- Generic Mach3mill

The Solidworks has the SAME settings (from what i can control) but is NOT named the same (no G43.cps). But Solidworks does not offer the same POST from the list of available. So I do not see "Mach3mill-G43.cps- Generic Mach3mill".


-Jason

[ger21]

There's much more to the post then the options they give you. A large portion of it are not user configurable.

[CROSSHATCH]

Sure, I agree now since I am only able to match the options of the POSTS but cannot change all of it, the embedded "hard" stuff.

Can I bring the POST (if I can find it) from Inventor to Soldiworks folder? Is that possible...?

-Jason

[mactec54]

The Inventor post provides this line: "T5 G43 H5 M6" which has not caused any issues.

The Solidworks post puts G43 on a different line:

T4 M6
(ER32 COLLET)
S6000 M3
G54
M8
G0 X-0.3648 Y-5.2405
G43 Z0.6 H4


All I know is that my machine runs correctly with how the Post comes from Inventor but does not do so with the Solidworks post.



Ray- I attached both POSTS to show that I am using similar/same settings. Except, Soldiworks keeps inputting G91.1 and adding G43 to separate line which is causing my machine to not function accordingly.

Regards,

-Jason

What you have in this post for G43 line is the correct way to use it, Mach3 supports it just like this, as do most CNC controls
If this is not working for you put a G90 in the line before

G90G0X-0.3648 Y-5.2405
G43Z.6H4

[SCzEngrgGroup]

The source for the posts in HSMXpress is in the posts sub-directory of the HSMXpress install directory, which is normally C:\Program Files\HSMXpress.

However, I think you've reached at least one incorrect conclusion. The G43 line you seem to think is a problem should not be a problem. I think you'll find HSMXpress always does a G43 BEFORE each toolchange, and the one you point to comes after the toolchange, making it both redundant, and harmless. You are not posting full programs, so it is impossible for us to figure out what your real problem is.... How about posting the Solidworks file for the part you're having trouble with, and telling us the exact POST you're using, then maybe we can help.

Regards,
Ray L.

[CROSSHATCH]

Hi Ray,

For some protection, I am not interested in posting all my code or model.


Ok so perhaps the G43 is not the problem. However, because it was a little different then my "qualified" G-code, I was looking for things out of place.

I just don't know why the machine is traveling up in the Z-axis a few inches and starting the cut from this elevated plane. So if I were to touch off the top of the stock, for some reason it would travel up, reset and clearly never make contact with the material.

I have another test code, so I will cut some air today and see how she responds.

-Jason

[CROSSHATCH]

Ok, so I got into the shop and edited the code.

Per Ray's response, I added G43 H# to my toolchange line. I did this for all appropriate tool numbers and deleted G91.1 from the beginning.

I ran the code in air and everything worked as it should. I suppose it's not too bad to edit the code and know what to look for etc...

Regards all,

-Jason