cuts the wrong size

[Gerry A Brown]

Hi Everyone,

I am doing a job for a customer that has prepared the files with Aspire. The files require slots & holes cut to an exact size and I find the sizes are not coming out correctly. Interpolated holes are under size by .005" to .01" and the same with the slots. Is there a calibration I can apply to get the cuts to cut the size drawn?

I own Aspire & do the tool-paths for the file & do the Post P myself.

Any help would be appreciated.

Thanks,
Gerry

[Scott G Vaal]

Gerry,

Add a G07F5 to the beginning of your posted programs and see if your holes are then correct.

[Gerry A Brown]

Hi Scott,

I will give that a try.

Thanks,
Gerry

[Gerry A Brown]

Hello Scott,

I did a few test cuts
1. a interpolated hole drawn at 1.05" cuts at 1.025" with .5" cutter
2. a slot drawn at .375 wide cuts at .3615" with .25" cutter
3. a slot drawn at .25" wide cuts at .247" with .25" cutter

This is with the G07F5 in.

I have attached the NC file so you can confirm I have inserted the command properly.

Thanks,
Gerry

[Scott G Vaal]

Hello Scott,

I did a few test cuts
1. a interpolated hole drawn at 1.05" cuts at 1.025" with .5" cutter
2. a slot drawn at .375 wide cuts at .3615" with .25" cutter
3. a slot drawn at .25" wide cuts at .247" with .25" cutter

This is with the G07F5 in.

I have attached the NC file so you can confirm I have inserted the command properly.

Thanks,
Gerry

Gerry,

Looks like your CAD/CAM is applying comp for the tooling, which is fine. However, did you actually mic your tools and see if they are under the nominal sizes? In my experience, the tools we get will not be exactly the nominal sizes. Might want to check this first. Also, are you possibly cutting too fast for the tooling and material (500ipm may be too fast for that arc radius and 3/4" material)? Also, it looks like you are doing a climb cut on the circle and the wide slot which would deflect the tool away from the finished edge. May try a conventional cut instead. If your CAD/CAM is capable, you may want to output the arc(S) as actual arc commands (G02 & G03) rather than the short G01 line commands that your program is doing (a series of short non-tangent line moves approximating the arc). G2s and G3s have automatic feed rate reduction applied based on radius and machine kinetics (but still may not reduce it enough for the tooling and material combination). By the way, the G07F5 that you have is needed and is in a good spot in your program.

[Gerry A Brown]

Hi Scott,
I'll give all your suggestions a try keep you posted on the results.

Thanks,
Gerry

[Brad McIntosh]

Scott,

If I am not mistaken, I believe that Control Nesting usually writes out NC code that turns OFF smoothing via a G07F0 call. (The default after a NC reset/HOME is G07F50 I think ??) Perhaps Gerry should try a G07F0 in place of the G07F5 suggested?

Just a thought.

[Gerry A Brown]

Hi,

I have been away from the shop so am a bit late responding.

Brad thanks I will try that. I have not tested any of the suggested mods yet but will post back with results when I have had a chance to do so.

Thanks,
Gerry

[Gerry A Brown]

Hi,

I have worked through this trying all the suggestions. I get good results doing conventional feed with the G07F0 code. I have modified the Post P to insert this command and it all seems to work well. I have not got the Post P to output arcs yet but will pursue that as time permits.

Thanks to everyone for their help on this,

Gerry