Laser Cutting tolerancing!

[var10]

Hey Everyone,

I have silly question to ask. I have blank plate to be laser cut which has funky shapes and 4 holes.

One of the key issues I always face is very tight tolerancing due to the industry I am in. I have ordinate dimensions as shown. My supplier rang me and told he can't do +/-0.1mm even with a laser cutter (he can actually but he will be facing a lot of rejects which he can't afford and fair enough). So I have checked all the affecting parts and I should be sweet to increase them to +/-0.25mm.

Because I have ordinates I am having this question - could this happen where dim=5.00mm is 4.75mm(with 0.25tol) and dim=104.00 is 104.25(with 0.25tol) I know that I have to accept this if this is what I get, but my question is will laser cutting equipment offset holes in opposite directions from where it is meant to be (I imagine they start at a virtual x,y,z (0,0,0) and if the offset happens by +.15mm in y direction, all the dims would be +.15mm in y)?

Am I right?

To clarify more the dim=77.00 with tolerance can be either 77.25 or 76.75mm but this is not the case for ordinates.


Any help is much appreciated.

 

[MikeHalloran]

Don't talk to a cutter about offsets. The word has a special meaning in the CNC world, and it's not what you think it is.

A tolerance of .25mm is unnecessarily loose.
0.1mm is a bit on the tight side, but 0.15mm +/- is probably achievable.

The problem is not with the cutting machine's controls, which are capable of normal CNC resolution.

The problem is deciding where the edge of the cut is when you inspect the part.
If you look at a lasercut part under a microscope, the edge looks like it was made by drilling adjacent holes to remove material. ... which actually is how the lasercutter works, blasting tiny holes through the material, right next to each other. So if you use a sharp or small ball probe, the apparent edge is in a different place than if you use a flat or large ball probe.



Mike Halloran
Pembroke Pines, FL, USA

 

[Walterke]

You should specify the center-center tolerance between the holes if they are important.

@Mike: Depending on the thickness of the plate (which the OP failed to mention), the edge should be fairly smooth, or at least smooth enough to not interfere with the tolerance.
Again, however, I think the distance between the holes is usually more important than the distance from the edge to the hole.

NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

 

[ornerynorsk]

As with any process, don't call out tolerances any tighter than absolutely necessary. This just adds unneeded cost.

All of the talk about specific capability of holding this tolerance or that tolerance is pointless because the material and sheet thickness have never been mentioned (unless I have suddenly gone blind).

0.1 mm location and size is certainly achievable with certain materials, but would be out of the question with other materials. And, of course, this depends on the vendor's machine and what they feel they are capable of, as well.

We use on the order of 250 tons of laser cut flats and tubes each year, mostly HSLA varieties and 1020/1026 carbon steel from 1mm to 6mm thickness, and our vendor routinely holds +/- 0.15 on nearly everything.



It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

 

[var10]

They are 2.3mm thick and made from Al2024-T3. Sorry forgot to mention this in my original post. But yeah I see what you mean.

It also depends on what tolerance applies where. My supplier told me he can achieve tight tolerances with holes and have to ease it up a bit with periphery as the work piece can move during the operation (very slightly). Any other considerations that I need to take into account during laser cutting, please share.

Thanks

 

[SceneryDriver]

My laser cutting vendor routinely holds ~0.15mm (0.005") tolerances with no problem in steel up to ~10mm (0.375"). He said he can hold tighter tolerances if asked, but cutting would be slower and thus more expensive. I've always sent him DXF files with my lines drawn EXACTLY as large as I want my parts / holes to be. For instance, if I drew a hole at 0.500", I was told to expect a hole between 0.497" and 0.503"

How accurate to you really need to be? If you need a super accurate hole size, ream it. Otherwise, oversize your holes by a few thousands of an inch and you should be fine.


-SceneryDriver

 

[SceneryDriver]

I just saw that you're cutting aluminum. Not sure of the exact behavior of the alloy you specified, but in my experience aluminum cuts slightly less "clean" then steel. And I do mean SLIGHTLY. Holes might be a little less clean; have your vendor cut a sample for you and chat with him about your needs.

My vendor has always been good at taking care of me if I put notes on my drawings about particular holes needing to be extra tight tolerances, etc... For instance, he'll even start the laser pierce at a specific spot if I ask, so it will be covered by weld in the finished assembly. Your vendor should be able to work with you. If not, probably time to find a different vendor.

I'll assume that by your referencing metric dimensions, you're not in the US. I have a good laser cutting vendor in Illinois if you're interested though.



-SeneryDriver

 

[KENAT]

var10 - I'll back up what Walterke says. It sounds like part of the problem may be your dimensioning scheme, I'd consider tweaking your dimension scheme to meet your functional requirements while allowing for the maximum 'tolerance' possible- making sure it covers that from the process capability.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​