Cut order / toolpath sequencing - wish list

[3DCNC]

Hi Vectric

Love my Aspire software.

Is there any plans to implement some sort of way of being able to manually tell aspire the order in which to cut/engrave/pocket profiles within one machining operation.

At the moment to do this I have to apply a machine operation to each profile in a job. In other packages they call it "cut order" or "toolpath sequencing " . It would be nice if it initially cut the profiles in the order that they were picked. ( Have the option to go back and edit)

Mark

[capnl]

Hello Mark,

the cutting sequence is decided by you and can be selected in Aspire......

Say you have an object to be cut in multiple toolpaths with different tools you can save the toolpaths for 1 tool as 1 toolpath and save the second and third path as such.

When a path is generated in Aspire you can change the sequence in the row of paths, it is much wiser to arrange things here (you can preview the result) instead of arranging the sequence while saving the paths into 1.

In this job (namesign for the location I am currently moving my business to) I did just that:



1)
4 toolpaths were generated for a 60 degree 6mm V-bit
- (profile) on the line of the rectangle outside the text with inside curved corners to a depth of 6mm
- (vcarve) the blue colored text
- (vcarve) the gold colored text
- (vcarve) the white colored text
the paths were selected in this sequence and saved as one path and by winpcnc executed in the same sequence.

2)
this was followed by 3 paths for a 5mm endmill
- (pocket) 9 mm deep from the rectangle with curved corners to the outside of the piece (drawn a rectangle there too) tool-stepover of 80%
- (drill) to create the 4 5mm dia holes in the corners starting at 9mm to full depth of material (24mm) peck dril, peck depth 3mm (=pass depth of the tool) - retract gap 5mm
- (pocket) of 10mm dia (with same center as the 4 holes) starting at 9mm depth and a depth of 5 mm

3)
After that is was necessary to have a profile outside the rectangle with curved corners to clean the transition from angled to straight of the outside upper part of the piece.
For this I also used the 5mm endmill.

4)
At last there was a profile again with 5mm endmill on the outside square to release the piece from the material.

NOTE: it is not always this easy, sometimes you have to have more toolchanges but there is some kind of logic-thinking to make it as easy as possible.

I completed this piece with only 2 tools and 4 toolpaths to be executed by winpcnc.
paths # 1, 2 and 4 were generated at the design-pc, #3 was generated "on-scene"

here is the result, just bare wood clean from the cnc machine




any questions ?? do not hesitate to send me an email or PM
btw: 1" = 25,4 mm

Cheers

John van Gent
DRW-Holland
Zuidland - The Netherlands

[dr_when]

the order in which to cut/engrave/pocket profiles within one machining operation.

If the key phrase is one machining operation, you cannot change the order. John was talking about arranging the different toolpaths I think. I think there would be times where changing the order within one toolpath would be handy because Aspire's optimizing is not always what you may want.

[capnl]

Hi Bob,

there is a way to overcome this (if I see correct)

in this sample we create a shape that is (hand)-nested 12x



The pieces are numbered (by us) 1....8 from bottom left to right 9.....12 top right to left,
in our mind the most effective solution is to machine part 1...12 in this sequence however Aspire is doing this differently and calculates the sequence: 2-4-9-3-11-1-12-5-7-10-6-8 (follow the red lines)

We can only overcome this by calculating each shape one by one and saving all paths to 1 toolpath in the sequence that we want it to be executed.
If this is really the most effective way I do not know, Aspire keeps in mind the startpoint of each shape etc.
When we arrange the sequence ourselves I do not know if there is any profit timewise because the time we think to win by machining our sequence is lost by us calculating the 'most effective way' of machining...........

correct me if I am wrong.
(I am only human )

John

[dr_when]

John,

I follow you and that makes sense. Especially the part about the time it takes to optimize ourselves in which the time could be spent cutting!!

[3DCNC]

Thanks for the responses. I think Aspires optimisation is good enough most of the time. It sometimes becomes a problem when you have multiple shapes nested within other shapes.

If you have a production job where the same shapes are being cut , it helps to be able to edit the sequence your self to save cutting time on your machine. Some times you can save 5 min of cutting time on a board, which does not sound like much until you have 12 to cut.

[ckurak]

And then there are those of us who do not have vacuum hold-down. So, the order of machining is particularly important. For example, if you cut out all of the parts around one in the center, then that last part to be cut (the center one) will most likely fly around loose on the table.

So, we do what John does: toolpath each part individually on the final pass (onion-skin pass) then save them to the cutting file in the order we want to prevent loose parts.

[3DCNC]

This could happen even if you have vacuum hold down. Some peices are too small for the vacuum to have any effect. Haveing to put tabs on many peices is not always feasable .

[gravirozo]

hi

all vectric program generate conturing, as the inside part first... for example cut "o" letters the program cut first the inside of "O"s ... the next condition is the "shorthest" distance part to part...

and if you have a special series, there already worth to spend time to make an own order... my experience is after i used other programs, i did set always inside>outside and the shortest distance between parts..to cut down the machining time.... because this two condition is important... and vectric has this settings...

for thin material, without vacuum, i use to be make "holes" with the router first between part..for extra screws.. sure the thin material don't "fly up"....

also you can cut time in case large pieces to relocate start points.... (available in node edit function)


thanks
viktor

[3DCNC]

Hello Victor

I have been CNC cutting for the last 4-5 years( not that I claim to know evrything) - I learn something every day.I appreciate the responses from anyone. I already use those functions/methods , but I still feel it would be very good to be able to set the sequence of the toolpaths . Most highend CAM systems have this option for when the automatic one will not work.

This is one for my wishlist.

many thanks

Mark

[gravirozo]

hello mark


yes i know other programs has this... i used it... however i just missed always something from other camprograms... that's why i used more type program at time... with vectricprogram... i use only this... need no outside help... and i trust vectric, they wont stop, they will develop more convenient function... probably this feature will come tru in the future..
i'm sure they have already surprize in the next versions... and this feature is in line in order... only question how many more important thing they have before this...

i like this forum.... from all around world people are here...

thanks
viktor