Please help with these pockets

[fraction.gp]

I have tried several tool path types including Spiral, 3D Pocket and Scallop. I am not getting anywhere - all have errors or do not reflect the geometry of the pocket.

They are all spherical dimples with a radius on the edge.

Say 55 diameter and 12 deep.

I need help with the options within the chosen tool path type to obtain the desired results.

Issues include, amongst others;

Tool path not cutting out centre of pocket.

Please see screen shots.

Would to be good to have screen shots of the relevant screens showing all correct options.

Hope someone can help.

Kind Regards

[seth.madore]

This might be related to your settings, either in the Setup or the toolpath itself. Would you be able to share your Fusion file here?
File > Export > Save to local folder, return to thread and attach the .f3d/.f3z file in your reply.

[fraction.gp]

Thanks Seth

Please see attached

[a.laasW8M6T]

Hi

Have a look at this video where I jump in and run through a few things that may help you out, File attached too

[fraction.gp]

Seth

I also tried using 2 pocket paths = one rough, one finish.

With pocket 2 I need the best finish possible including all of the small top radius, not sure if this is the best way - see crazy tool paths.

The tool I was using for roughing is from ISCAR - FFT3 W X M T 030206T (no spaces between first 4 characters - gave an error without them)

Please see file attached.

Many Thanks

[a.laasW8M6T]

Hi

If you go to "More Info" on the Iscar page:

You get the info with the programming radius:

So you would define this as a 10mm Bullnose with a 1mm corner Radius

(3D)Pocket is a roughing toolpath only and should not be used for finishing

"The best Finish possible" is still arbitrary, do you need a 1.6µmRa finish? or do you need a 0.2µmRa finish?

A cusp height of 0.006 should get approximately a 1.6 ra finish and 0.003 should give around 0.8ra and so on.

I think spiral should give you a decent result with a fine stepover

You could additionally run a blend toolpath for the top fillet if needed.

See attached

[fraction.gp]

Thank you Seth & Andrew

I will be looking into your answers in detail over the weekend.

I did notice when I opened the f3d file that there was an error - passes were discarded,,,,,,,,

I wasn't sure why.

Kind regards Jeremy

[a.laasW8M6T]

Hi

This is not an error, but a warning.

Its just saying the toolpath cannot get to the bottom of the pocket because the tool is too big.

There is only minimal extra stock left.

You could run a semi-finish pass with the ballnose using spiral and 0.1mm stock to leave before running the final finishing pass

[fraction.gp]

Andrew

Thank you for your video and file, they were a great help.

Can  you answer the following questions as I have one chance to get this right.

The second part is basically the negative of the first part with a 3.01mm clearance. The material is 350 grade steel. The finish is a priority.

1) Can you have a quick look at the file attached to see if there are any errors (simulation seems ok).

2) My pattern has a folder and pattern with "active buttons". What do they do and how are they deselected? How do you deselect them and how do you remove the folder?

3) The finishing tools are; ISCAR EB060A08-2C06 IC903 and ISCAR EB100A13-4C10 IC900. Many of the step overs and step downs are very small, should i be concerned about rubbing remembering that surface finish is important?

Once again many thanks for your help and Seth.

Kind regards Jeremy

[a.laasW8M6T]

Hi

This side is a bit trickier for a few reasons

See video and file

[fraction.gp]

Thanks Andrew

I will be looking into this shortly, however, I will have to go with a 10mm cutter, not a 25mm cutter as I don't have one.

Do you see any issues with scaling this from 4 positive and negative dimples to 240 (possibly in 4 groups of 60)? Do you think I will get 1 part (60 dimples) without changing or rotating inserts?

King Regards Jeremy

[fraction.gp]

Andrew

Further to previous reply;

I have a 20mm cutter that uses APKT 1003PDR HM90 IC908 inserts.

Could I use this?

Regards Jeremy

[a.laasW8M6T]

Hi

Easy solution to not having a 25mm cutter is to just get one 😀 it will not only be way faster to rough the bulk material it will help the inserts in the 10mm last longer as it doesn't have to do so much work

You could be pushing it getting the 10mm to last that long.

Assuming you are using the IC808 grade I would go on the lower end of the surface speed and the higher end of the feed and DOC, this will help the inserts last longer.

Seems the optimal here is the higher depth of cut with slightly lower feed per tooth

Make sure the tool stick-out is to a minimum and using a short rigid tool holder

Ideally use a strong air blast directed at the tool, or through tool air if you have it.(Although Iscar does say you can use coolant with these inserts)

That's giving a 36 min cycle time using the 10mm for the entire pocket, you could probably get double that time(Maybe triple) on one edge of the insert but a would be doubtful you would get 15x out of one edge.(Iscar Reckons 80 mins on one edge)

If you do want to stick with the 10mm you could program the roughing in several toolpaths at different heights with a compulsory stop(M00) in between them to allow you to index/change the inserts.

As for the finishing to achieve optimal tool life the finishing tool should be removing minimal material, say 0.1-.2mm with no large cusps.

So you want to do a semi-finishing toolpath with one tool leaving some stock and then finish with another tool.

Again getting the tool to last will be a matter of getting the Feeds and speeds right, not soo fast that the tool wears out prematurely and not so slow that you get a poor finish.

What that is exactly will need to be somewhat determined by experimentation.

[a.laasW8M6T]

That APKT cutter will work but will be very slow, especially hanging out 70mm from the holder, those APKT are very old tech inserts.

[seth.madore]

---

@a.laasW8M6T wrote:

..those APKT are very old tech inserts.

---

Yes, yes they are.

[fraction.gp]

Thank you so much for your help Andrew and for the time you have spent. It is very much appreciated and I have learnt a lot - still just a beginner.

I will buy a 25mm cutter (FFX4 ED25-4-060-C25-04) - I think the program run times will be way too long, particularly when I run multiple parts with 60 dimples.

Just one other thing;

What do you use for calculating your feeds and speeds?

I used to use a program called GW Wizard which I thought was ok.

It took into account things such as machine rigidity, tool stick out, chip thinning in 2 directions and other things.

However, it required a link with the "writer" much like Fusion. It was a one man show and he has recently passed away which leaves me with nothing except manufacturers recommendations.

Kind regards Jeremy

[fraction.gp]

Andrew I have looked at ISCAR tool advisor - Are these values good if you can't add your machine specifics?

Regards Jeremy

[a.laasW8M6T]

Hi

I use the FS wizard Pro app on my phone

https://fswizard.com/

Which has a desktop version that has more features

https://hsmadvisor.com/

I don't use the desktop version myself, I find the app is sufficient for what I do.

Also I only really use it for Solid carbide tooling like endmills.

I find for Insert tooling you are better to go with the manufacturers calculations as the Insert grade can have a large affect on the cutting parameters.

The Iscar tool advisor is pretty good

There is an element of experience also that influences my choices that a calculator may not always take into account

[a.laasW8M6T]

You don't have to get all the details 100% to get a result.

These are often starting values and you will need to adjust parameters depending on your particular machine and work holding/tool holding anyway.

Sometimes the part is flimsy and vibrates so you need to use smaller depths of cuts. Sometimes you have a very rigid setup and you can go to the higher end of the parameters.

Like here, 50mm Feedmill, 1mm doc 35mm stepover, 1mm per tooth feed.

That's sort of mid range for this cutter, could go more on the feed and DOC, especially on this Big BT50 Bridge mill(52Ton machine)

Similar parameters but on a lighter  BT40 machine, with a much longer arbor, still ran pretty good, Chip evacuation became problematic though

[fraction.gp]

Thank you so much Andrew.

I will be finishing the two test programs over the next week or so and hopefully organise a 25mm cutter.

My machine is only BT40 (1000 x 500).

I will let you know how I go.

Kind regards Jeremy