[KSPATZ]

Hi all,

Here I am again for searching a solution.
Enclosed picture show the job I have, but the resilt always is very bad!
I tried it as single step milling (full deep) and micture between 90degr and box milling. I believe I tried over 20 different jobs with different routes, but I don't get a succesful result. Result you also could see in picture.

Could help anyone for best way to get a perfect resul?? Or does anyone a idea for the failure I make always??

Material is Al, tools you could see in JPG (tools are new!).

Hope for your soonest help!

Kind regards
Kersten

[williamsmotower]

What type of machine is this?

What is your final pass cut depth?

[Dan B]

I've found that when cutting with a chamfer tool it's best to run it with a slow feedrate. I've had good success between 200mm/m and 300mm/m. I notice you are programmed at 600, so you could try that.

Dan

[keebler303]

Make sure its a machinable grade and heat treat of aluminum, like 6061T6 or similar. Also looks like you need an air blast or flood coolant as the chamfer is all scratched up from recutting chips.

Matt

[HuFlungDung]

There appears to be some horrible dragging and scraping going on where the chamfer meets the floor of the pocket. From your tool description, your chamfer tool has a zero tip diameter. Unfortunately, when a chamfer tool has a zero diameter tip, then it also has no cutting edges and no chip gullets at the tip, hence the mashing of the workpiece.

You need to use a chamfer tool with a reasonable tip diameter so that proper cutting action has a chance to occur.

[br1]

Is this a climb cut or conventional cut, I would think a climb cut as a final pass would clean that up, and also as mentioned using some sort of coolant.

[Dan B]

I took another look at the path in madCAM, and it is a conventional cut. I didn't notice that when I first looked at it. Good call BR1!

Kersten, I think if you take all these suggestions and apply them you will have much better results.

Hope this helps,

Dan

[KSPATZ]

Hi all!

A lot of thanks for your help!
YES - best success we reached first with climb cut. Quality was much better.
Then we decrease the speed - it also was helpful.
Furthermore we bought a vacuum table to adsorb any vibration from material - this is always under test, but looks more and more better!
Finally I will buy a chamfer tool with 2mm diameter tip, to have best possible result!

Finally a lot of thanks for halp to all!

Kind regards
Kersten

[Dan B]

I'm glad to hear it worked out.

Dan

[KSPATZ]

Hi Dan B

In last post I wrote that quality is better than before, but it was not perfect! I found special champfer tool (45 AX1) to realize a better result (tapered end mill center cutting).

http://www.tce-tools.nl/PDF_catalog/...A16/fam220.pdf

I have defined tools in madcam, but I don't have any idea to use it.
Problem: when I would like generate a milling path (depth 2.5mm) by conture with inner direction, no path will be generated. To generate path I think always dim "d2" will be used (it is 16mm at this tool). If pocket have width smaller 16mm - no path will be generated, but the 16mm is end diameter in "height" 7mm (dim "l1").

The enclosed picture shows our result today (2 tools in 2 paths), but we used trick to made this. We used for milling path tool end mill with diameter 2mm + inner conture, total milling depth 2.5mm with steps of 0.6mm. The result looks fine.

To mill the champfer the problem is solved, but it is not the best way not to use the correct tool in simulation.

Does anyone have better way to see also the result with our new champfer tool in simulator???

Kind regards
Kersten

[svenakela]

Kersten,
Make a screenshot at your tool dialog and your contour settings dialog and post them here.
This is a handling/tool/machine issue and really not related to the software (ie. you'll get the same result with any software). If you post the dialogs it's much easier to help you with the settings.

[KSPATZ]

Hi svenakela,

thank you for help!
Enclosed you could find our adjustments.
Under using this values for bevel tool no path will generate! Only when tool diameter "D" is lower or same as 10mm a path will generate!
This I don't understand!! Where is my failure in understanding and adjustment??

Kind regards
Kersten

[svenakela]

Ok, I tried the same thing and got the same result. If there's no logic explanation it's probably a software defect that sneeked into the latest version.
I have already reported it to MadCAM.

The solution for you right now could be to make a toolpath with wrong values in the tool dialog. You can actually create the path with a straight 2 mm end mill. The simulator will be wrong, but the real world cut will be correct.

Regards,
Sven

[KSPATZ]

Hi Svenakela

great- that you have same result!
Your proposal with straight 2mm end mill we used to make the result you could see few topics before!

Kind regards
Kersten