Canned cycle face turn problem

[Wiseco]

Hi,

I tryed to do a canned cycle face feature and the code goes weird. You will see that my setup UCS is align with the backface of my rod, which is turned in a precedent setup. See the last pic.

First pics is my curve

Second pic is the code in canned cycle. See the coords before the g72? The z-coord is suppose to be something like Z3.75 but it code Z0.1.(take in consideration that I have canned clearance of 0.1 in X and Z.)

Third pic is the code without canned cycle. The starting coords looks very good in this patern!

I have knowledge on customizing post-process but can't find a way to correct this.

Ok, you will tell me, why would you spend time to correct something instead of using a simple feature? The reason is I customize my post-process to work perfectly as I want with my Haas lathe so I would not have to correct anything in the code in any feature. Most of the post-processor is done except this part that is a pain in the ...!

[lakeside]

Your Face Would Be Z 0 If You Touched Of Your Tool There ALSO I SHOULD ADD THAT I HAVE NO KNOWGLE OF THIS SOFTWARE

[Wiseco]

No because the setup UCS isn't on the right face of my part. Is on the left face (back face) of my part which is turned before.

[lakeside]

I Real Can't Help I Don't Know This Software

[Wiseco]

Part have been drawn with Catia and the UCS of the CAD is completely on the tail of the part so I think it isn't a part of the problem.

But I have tryed to translate all UCS to be with the Setup UCS and it does nothing to the code so...

Thanks for trying!

[hilldf]

Wiseco,

I have found I need to set my Z Clearance to the amount of stock I need to face off when using canned cycles.
I always program with Z Zero at the opposite end from what you have. So, if I need to remove .30 from the face, using a canned cycle, I would set Z Clearance to .30.
I do not know if there is a better way, but with this method I have been able to use all canned cycles in FeatureCAM with no edits on Fanuc and Okuma controls.

[miljnor]

Canned cycles always seam to have problems. I don't recomend any of them.

[Geof]

Originally Posted by miljnor Canned cycles always seam to have problems. I don't recomend any of them.

Yes when you are stubborn and don't want to edit on the machine. The G71, G72 and G70 cycles on the Haas lathes are great time savers.

[Wiseco]

Thanx hilldf,

I put my setup there, at the backface because I use a .25 spacer between the chuck jaws and the backface of my part. This way, I can avoid chattering as the tail of my part is only 5/8. Also, all my tools Z offset are set .25 of the front of my chuck jaws. So when I have to make this kind of job, I put work offset to Z0. If somewhere in the job I didn't have enough stock to setup my work to be able to make the cutoff, I can even turned the tail. And when I setup the second part of the manufacturing, I just enter a guest lenght of the rest of the part to be turned. So I just have to enter that lenght in the start point of the canned cycle and the program make the part.

This way, I can setup stocks quickly without having to measure accurately how much stock lenght that I have.

I will try with the Z clearance, I think it will do the job.

Yeah I saw that canned cycles are tricky with featurecam and their post-processors. I'm trying to customize my post-processor to correct this. I want to have good output codes out of featurecam so I don't have to edit on the machine to save time as we made many different parts.

[jimwymz]

Wiseco,

Many Posts have a "Canned Set of output Code" at "Beginning of Tool",
Perhaps yours always assumes That all Lathe work Starts at the Finished Face.
(as several here have suggested... I understand why you are setting at the Locating Surface, I usually set at Face first op and at Locator for second op, Preferable to be easy for set-up and if Possible I set up so program reads like the Print), Sometimes I set 2nd op at Locator and shift the Work Zero in the Plus Z direction by the Finished Length of the Part.

No Matter which way you do it THE OPERATOR MUST HAVE CLEAR DIRECTION AS TO WHERE TO SET ZERO!!!

When you set ANY work coordinate In your Post and use same place in Space on the Machine Tool then the Coordinate's would appear the Same values (as they sort of appear in your Posted and Manual code).

Between both Prg's I see the Big difference in your starting Point only, All other Z moves In the Posted G72 cycle and Just after N60 are correct.

In any Canned cycle I do, the XZ position before Start of Cycle IS ALWAYS the same in the Line following the END of the Cycle.

Look in your Post at the Tool Start up section, I'll bet it has the X position Looking at the Stock Diameter Variable, While the Z is Probably Hard-coded at Z0.1!

JimW