Saving tool setup in Winmax

[Captdave]

I hate the way Hurco doesn't save your tool set up independent from the program like most controls do. The manual mentions setting up tool templates but has no details as how to save, load, edit the file. I'm sure its a simple process if someone could enlighten me as how to do it.

[glovebox20]

I know the feeling all to well.

If you have the Tool and Material Database option, I belive the Tool length is stored on the "Machine" and not the program along with the material and speed and feeds for that tool.

Import (Winmax)/ Restore (Ulitmax) functions

However, if you do not have Tool and Material Database option, your current tool setup is lost when you read a new program in to the memory. You can get around this. If you are running program "Mill Hex" and want to run a new program named "Thread Mill", while saving current tool/part setup, Use the "Import Functions/ Restore Function" in the main Input screen. Select "Part Program" and make nothing else is highlighted. Your file directory should appear and find "Thread Mill" program and press enter. You still have the same tool/part info setup, but it replaced your "Mill Hex" program info. with the "Thread Mill" program info.. Your programed is still named Mill Hex. You can import Part Setup,Tool Setup, Program, or Parameters one at a time or all together or any other combination at the same time. On the Ulitmax control, your are limited on your combination's.


Tool Templates:

Let's say I drill alot of 1/4-20, .251 Ream, 1/4 C'bores, 5/16-18, .3135 Ream, 5/16 C'bores, holes plus some milling and Face cutting.

First, Make new program with all your tool set up info. (leave tool offset blank)

Then go the part program and make a block Containing All your Drill cycles with no locations. You may what to make a block for each size of holes. Write this program to your hard drive and save it with a familiar name so It can be found quickly. (sample:" ^CRS" for cold rolled steel)

How about that, you received another print with some 1/4-20, .3135 Ream, and 5/16 C'bores holes. That's easy! 65% percent of your work is already done. Create a new program names "Base Plate". Now use Import/Restore Functions to read your "^CRS" template program info. you will want to restore your Tool and Program info. Now Program your part by adding your necessary hole locations and delete All the unnecessary info you don't need. Now you many want to copy your block a few times and delete the extra hole operation's so your spot dills all holes first before changing to the next tools. Now add a few blocks to face the top off and mill the part to length or what ever you need to do. Assemble All your tools and touch them off and pick up your X,Y,Z zero. and run the part. Remember to draw the part out on the Graphics screen and look at a couple of different views to make sure your tool path looks right and SAVE your program to the hard drive. Nothing worse that having the computer lock up so all your offsets and program are gone when you reboot it.

What? Another print, only with .251 Ream, .3135 Ream, 5/16 C'Bore. Sweet, 85% of the work is already done. Save your current program to hard drive (Base Plate). Import/Restore your ^CRS program. Only the program!! or your offsets will replaced to nothing and you have to restore your offsets from your last current program or touch them off all over again. Again, add the locations for the holes and add a few mill blocks as needed to complete the part and delete all unnecessary info. Assemble your missing tools and touch them off as well. Graph your program to make sure it looks right and pick up your X,Y,Z zero and Go (with cation of course) Rember to save your program again (Base Plate B?). Whenever you update your tool/ part offset you really should save the program to the hard drive as well so you won't loose your offsets.

This how I do it when I'm at work. The hardest part is keeping track of your offsets so you don't accidentally rewrite them by mistake. And ALWAYS be cautions when running your first part to make sure offset/program are good to go.

I believe with the Winmax Software, you can go to Program Review and highlight and copy a few blocks to your "Clipboard" than load a different program and paste those blocks into it in the Program Review page.

Look under Getting started with Winmax Mill manual 4-26 for the "Creating Tool setup Template" description, 4-43 for Import functions.


Hope this helps clears things up a bit.

glovebox20

[Advena_SA]

Try this, Start new program put all your tools in this program that you can think you are going to use, be it 20 or 500 of them, endmills,drills all the tools in your workshop etc. Now save this program as your tooling program. So whenever you now start a new program you go to the import screen and import your tools, and all your tools is ready for use

[Captdave]

Well that sounds easy enough, let me see if I can mess that up too.

[Captdave]

That work pretty well. Started a new program and had to use some different tools that were not previously saved, do I import them back into the tool program and if so will it over write the previous tool assignment, example tool 14 was a m10 tap but now its a 3/8-16, to keep it up to date?

[glovebox20]

You could do it that way if you wish.

I would open up your "tool program" and modify your changes and save it again. I like to leave the offsets cleared to "zero" in my tool program so if I import the too setup into another program, I'll be forced to update the tool offset to avoid unexpected tool offset errors.

Once i start touching off tools and making programs, I'll save my current program, and if I retouch or adjust any offset, I'll save the current program again to keep the offsets up to date.

So I have two programs, A Tool setup program with no offsets saved so when I'll starting from all over from scratch, I'll use that one for my tool set up. But, once I get the mill up and running, I have a Current program saved witch I'll keep importing my programs/part offsets into. If I need to run a different program, I'll import the new program into my Current program program or just rewrite over my program.

I'll even go one step farther, and have a program saved just with a particular part offset. When I'm facing bar stock down to size, I like to write my tool path from the upper right edge of the vise jaw (ex. "RH" for right side of vise). Then I'll create a facing program big enough to cover the part, Import my part setup from "RH" program, update the Z offset & go. Tip: You may want to set the Z offset to 99.000" in the "RH" program, so if you forget to update your Z offset, it should error on the positive side and not the negative side.

glovebox20

[Captdave]

That sounds like a better Idea all the way around. Thanks for the input.

[glovebox20]

Happy to help!