finish turning aloowance

[nigelbutlerSQ2QR]

hi

is there a way for the post processor to use the stock allowance on the finish turning?

i have also tried a generic haas and fanuc post but get the same results

the model and toolpath work as they should in fusion 360,its when it posts it out that the leave allowance disappears

ideally needed for semi finish passes,for now i edit the figures to suit

G0 Z-4.996
X73.72
G1 G41 X76.414 Z-6.343 F0.1
X69.1 Z-10.
Z-16.
G40 X64.9 Z-16.4
G0 X58.
Z10.

the x69.1 should be x68.7

[seth.madore]

The "Leave Allowance" should be passed through to the code. Can you share your file?
File > Export > Save to local folder. Return to thread and attach the .f3d file in your reply

Oh, what post processor do you need to be using for your machine?

[nigelbutlerSQ2QR]

as above i have tried a generic fanuc post,a haas post and they dont leave anything on the bore

the post i use is for a centroid controller that is similar to fanuc but it is exactly the same

looks like it is a post issue

[Anonymous]

Using few different posts, turns out it will leave stock if you select "in computer" compensation but not if you select "in control" compensation, Fusion bug.

[nigelbutlerSQ2QR]

thanks

doesnt help to control my bore size

ill manually edit it for now,ill have a look at the post processor to see if i can edit it

[Anonymous]

Not leaving stock when in control compensation is selected is a bug in Fusion not in the post.

Your tool is defined correctly but your setup is not, I simplified the task to one pass with few changes to set up.

Cutter comp is only applied to chamfer, compare two files showing in computer and in control compensation.

You are making 3 mm chamfer, 45 degree compensation for .4 mm tip radius is .234 (.0092 in) with slight discrepancy due to rounding off.

I made face of th part Z0 (model top), making facing and boring pass clearly shows only one place where compensation is applied, compare two NC files.

With radius and tip properly set in tool offset page of your machine, run in control compensation program in single block and observe "distance to go" at start of chamfer move, X and Z values will match those in file using in computer compensation.

So, cutter comp does not control your bore size, you do that using X axis wear offset.

2020-10-06 06_58_17-Basic 3-D Viewer - V1.0.0.45 C__Fusion_NC_1001.nc.png2020-10-06 07_14_31-Basic 3-D Viewer - V1.0.0.45 C__Fusion_NC_1001.nc.png

[akash.kamoolkar · Accepted solution]

Just to clarify this is a bug and we will be looking into fixing it.

Regards,

Akash Kamoolkar

[nigelbutlerSQ2QR]

i think your are mis-understanding where i am coming from

by using the stock allowance for a semi finish pass(not the final pass)you can find out exactly where the tool is

you will then run the same feature again without using the stock allowance to get your final size

if the tool is slightly out on the semi finish pass(thermal growth of machine,pre setter out,manually measuring tool etc..)then you will use the wear offset on the machine to alter the size

[nigelbutlerSQ2QR]

perfect thankyou

any chance you can have a look at doubling all the x axis sizes too so it reads like a lathe so we can see diameter on the simulation

[Anonymous]

---

@nigelbutlerSQ2QR wrote:

i think your are mis-understanding where i am coming from

by using the stock allowance for a semi finish pass(not the final pass)you can find out exactly where the tool is

you will then run the same feature again without using the stock allowance to get your final size

if the tool is slightly out on the semi finish pass(thermal growth of machine,pre setter out,manually measuring tool etc..)then you will use the wear offset on the machine to alter the size

---

I do semi finish and finish pass in many cases, first pass to measure and correct if needed and second to go to size.

Speaking of miss understanding, I pointed out the fact that bug is in the Fusion and not the post, after you stated that you will try to edit the post.

Also, compare your file to one I uploaded and check settings in setup of your file.

BTW, (ignore Fusion bug for a second), looking at your original file, leaving stock and doing spring pass will result in two passes on same diameter and because spring pass would not cut same amount of material as first pass, your measurement would be deceiving.

You want to do two finish passes of equal depth and same feed rate instead, that allows to repeat cutting pass under same conditions and your target dimension is more likely to be achieved without surprise deviation due to different cutting conditions demonstrated in your original file.

[Anonymous]

OK, disregard my post about cutter comp, I was under impression that you attempted to control bore size by adjusting radius value in machine's tool offset page.

[akash.kamoolkar]

FYI, this issue has been fixed in the latest update.

Regards,

Akash Kamoolkar